Oasys LS-DYNA Environment 8.1 VOLUME 3 ... - Oasys Software

Oasys LS-DYNA Environment 8.1 

VOLUME 3 : USER GUIDE 

Oasys Limited Version 8.1 

The Arup Campus Revision 0 

Blythe Gate May 2001 

Blythe Valley Park 

Solihull 

West Midlands 

B90 8AE 

Copyright Oasys Ltd.

Oasys LS-DYNA Environment: User Guide (Version 8.1) 

SECTION 

CONTENTS 

1.0 OASYS LS-DYNA ENVIRONMENT 8.1 

2.0 PARALLEL 

3.0 FILE STRUCTURE 

4.0 KEYWORD INPUT 

5.0 UNITS 

6.0 MATERIAL MODELS 

7.0 ELEMENTS 

8.0 RIGID BODIES 

9.0 CONTACT SURFACES 

10.0 RESTRAINTS AND CONSTRAINTS 

11.0 ENERGY DATA 

12.0 TIMESTEP CONTROL 

13.0 DYNAMIC RELAXATION 

14.0 HOURGLASSING 

15.0 IMPOSED MOTION 

16.0 AIRBAGS 

17.0 SHEET METAL FORMING SIMULATIONS 

APPENDICES 

APPENDIX A KEYWORD INPUT DECK EXAMPLES 

Page 0.1


Page 0.2


1.0 OASYS LS-DYNA ENVIRONMENT VERSION 8.1 

The version 8.1 of the OASYS environment contains the following main program revisions. 

LS-DYNA version 950.e 

OASYS PRIMER version 8.1 

OASYS D3PLOT version 8.1 

OASYS T/HIS version 8.1 

LS-DYNA version 950.e 

Version 950.e is a bug fixed version of other 950 versions. Version 950 is a major release from 

version 940.2 and incorporates many enhancements and new features. 

Major new features in LS950 are the inclusion of an imbedded implicit solver, which can be used 

to solve the springback calculation following a metal forming analysis in a seamless fashion. 

There are a number of new material models in this version and several material models have been 

enhanced by the addition of a viscoplastic strain rate option. There is a new option to set failure 

for all the solid material models. 

Significant enhancements have been made to the airbag contact (set nsoft to 2) and the 

performance of the other contacts has been enhanced. 

A detailed list of the enhancements in this version can be found in the version 8.1 release notes. 

OASYS Primer version 8.1 

Oasys Primer 8.1 is a major update from version 8.0/8.0a. This version contains a large number 

of new features and a number of enhancements to the existing features. The major changes 

include 

` Improved I-DEAS Master Series universal file reader 

Material database 

Bill of materials 

Spotwelder 

Contact penetration checker 

Ability to contact initial velocities, added mass, yield stress and density. 

Automatic massing up of the whole model, or groups of items. 

Automatic creation of ‘ZTF’ file containing additional data for D3PLOT. 

Output of PRIMER GROUPS to a D3PLOT groups file for use in post-processing. 

For more details on the new features available in PRIMER consult either Volume 1 of the version 

8.1 manuals or the Update and Release notes. 

Page 1.1


OASYS D3PLOT version 8.1 

Oasys D3PLOT 8.1 contains a number of new features and some enhancements to the existing 

features. The major enhancements include : 

` Improved blanking menu. 

` “Quick Pick” options for blanking, setting colours, transparency and colours. 

` Modified screen layout to improve ease of use. 

` Viewing of nodes from node to surface contacts. (via ‘ZTF’ file created by PRIMER) 

` Viewing of nodal constraints and restraints (via ‘ZTF’ file created by PRIMER) 

` Identification of *MAT_SPOTWELD beam elements (via ‘ZTF’ file created by 

PRIMER) 

For more details on the new features available in D3PLOT consult either Volume 2 of the 

version 8.1 manuals or the Update and Release notes. 

OASYS T/HIS version 8.1 

Oasys T/HIS 81 is a minor update to the version 8.0 software. For more details on the new features 

available in T/HIS consult either Volume 2 of the version 8.1 manuals or the Update and Release 

notes. The enhancements include : 

` New MINimum, MAXimum and AVERage functions. 

` Improved FFT function. 

` New WINDOW function. 

` Support for DEFORC, NODOUT, RCFORC and SBTOUT optional LS-DYNA ASCII 

output files. 

` Identification and labelling of minimum and maximum curve values. 

` Automatic generation of T/HIS command files from an ASCII input file. ( see FAST-TCF 

manual for more details.) 

Page 1.2


2.0 PARALLEL 

VERSIONS 

Two separate versions of LS-DYNA are currently under development for use on parallel 

computers; the PVP version (Parallel Vector Processing) and the MPP version (Massively 

Parallel Processing). The PVP version is a shared memory version and is available for use on 

most machines. The MPP version is a distributed memory version and runs on the Cray T3D, 

T3E, IBM SP2, HP and Intel Paragon machines. 

PERFORMANCE OF PVP VERSION 

The parallel performance of the PVP version of LS-DYNA is not linear with the number of 

processors used to solve the problem. At best it is expected that the current PVP version will 

show a speed up of 2.5 over 4 CPU's and that using more than 4 CPU's will not achieve any 

substantial gain. This drop in parallel performance is due to the large complexity of LS-DYNA 

meaning that it has not yet been possible to parallelize the whole code. 

The best parallel performance of LS-DYNA can be obtained on problems involving only a few 

element types, material models and contacts. In general a problem with many options, e.g. 

contacts, constraints, rigid bodies and airbags, can only be carried out in parallel 80% of the time. 

Table 2.1 obtained from Amdahl's law gives a rough indication of the speed up that can be 

expected in optimal cases. 

Parallel 

Fraction 

Number of Processors 

2 4 8 16 

75% 1.60 2.29 2.91 3.34 

82% 1.69 2.60 3.54 4.32 

95% 1.90 3.47 5.93 9.14 

RESULTS CONSISTENCY 

Table 2.1 - Theoretical Parallel Speed-ups 

When running LS-DYNA in parallel on different numbers of CPU's, in both the PVP and MPP 

versions, some results will differ. Not only will these results vary with the number of processors 

but they will vary if the same analysis is run on the same number of processors at a different time. 

The magnitude of these differences will vary with the type of problem, they can be so small that 

unless people check very carefully results appear identical. For most structural applications these 

differences are in the range of a couple of percent but for some applications some results could 

Page 2.1


differ by as much as 10%. 

Why do you get a difference ? 

When any calculation is performed the answer is subject to numerical roundoffs. Normally these 

roundoffs are not an issue but when calculations are performed over multiple CPU's the 

roundoffs change due to the operations being performed in a different order. 

Consider the following simple loop 

DO I=1,80000 

SUM = SUM + VAR(I) 

END DO 

One way to perform this loop in parallel on 4 CPU's is to break the problem done into 4 separate 

loops and then sum together the results from the four loops. 

(CPU 1) DO I=1,20000 

SUM1 = SUM1 + VAR(I) 

END DO 

(CPU 2) DO I=20001,40000 


END DO 

(CPU 3) DO I=40001,60000 


END DO 

(CPU 4) DO I=60001,80000 


END DO 

SUM = SUM1 + SUM2 + SUM3 +SUM4 

Due to the different operation sequence the value of SUM will differ between the single CPU and 

4 CPU calculations. If another variable, NORM, is now defined by subtracting SUM from a similar 

value the roundoff, that is insignificant compared to SUM, becomes more significant. If in turn 

NORM is used in another expression to divide another variable the results can be significantly 

affected. 

Page 2.2


Singular Behaviour 

Some events that are analysed, such as crash simulations, can exhibit singular behaviour as the 

panels buckle and contact each other, this leads to the spread of results that is often observed. 

When such an event is analysed using LS-DYNA, on a single CPU, the order in which the 

calculations are performed ensures that the program will always predict that each panel will 

buckle in the same way, leading to consistent results. 

If a complex model is analysed using the parallel version of LS-DYNA the roundoff errors can 

influence the local buckling modes of some panels. This leads to a spread of results being 

obtained for different numbers of CPU’s. Although all of these results may be valid it can be 

very confusing for users who are use to a single set of consistent results. 

OBTAINING CONSISTENT RESULTS 

To eliminate the roundoff issue for users LS-DYNA has significant work done to force the 

operation sequence for multiple CPU's to be the same as for a single CPU. Users are now offered 

a choice in the form of an 'accuracy' flag to control whether these options are used as they can 

have an overhead of between 5% an 20% depending on the analysis. This option is activated by 

setting ACCU to 1 on *CONTROL_PARALLEL, this is the default option in LS-DYNA. 

RESTARTING 

If a LS-DYNA analysis that was run using the parallel option has to be restarted, from a dump 

file, then it is advisable to restart the analysis using the same number of CPU’s that the first 

analysis was run with. Under NO circumstances should more CPU’s be used but less may be 

used with caution. 

The above section is based on the following paper : 

Dennis Lam, “Parallel Processing of LS-DYNA”, 3rd International LS-DYNA3D 

Conference, 1995. 

Page 2.3


Page 2.4


3.0 FILE STRUCTURE 

This section lists the file naming convention adopted by LS-DYNA 950e. The user does not 

have to set up the file names as these are handled by the OASYS_81 shell, which is described 

in Volume 2 of the version 8.0 manuals. 

Input Files 

The input file to LS-DYNA is given the extension .KEY, for an initial analysis and .KEY01, 

.KEY02 ... for a restarted analysis. Thus if the analysis root name is analysis_ralph_1, 

(the root name may be up to 70 characters long) then the initial keyword input file is 

and for restarts the keyword files are 

Output Files - binary plot files 

analysis_ralph_1.key 

analysis_ralph_1.key01 (1st restart) 

analysis_ralph_1.key02 (2nd restart) 

A number of binary plot files are created by LS-DYNA and the names of these files are made up 

as follows: 

root_name.typenn 

where :root_name is the analysis root name 

type is the file type and takes the following values 

ptf - complete state plot file (transient) 

thf - time history file 

xtf - extra time history file 

rlf - complete state plot file (dynamic relaxation) 

ctf - contact force plot file 

nn is the family number of the file, which is blank for the first 

member and takes the value 01, 02, 03 ... for subsequent 

members (upto a maximum of 999). 

Thus for the analysis given above the following files could be created: 

analysis_ralph_1.ptf 

analysis_ralph_1.ptf01 

analysis_ralph_1.ptf02 

Page 3.1


analysis_ralph_1.thf 

analysis_ralph_1.thf01 



analysis_ralph_1.xtf 

analysis_ralph_1.ctf 

analysis_ralph_1.ctf01 

The number of family members depends upon the frequency at which the data is written and the 

amount of data written for each state. A new family member is started when either the current 

member becomes full or a dump file is written. 

Output Files - ASCII 

The ASCII files produced by LS-DYNA are as follows. The general print out file that echoes the 

input data and gives the status of the job is given the name root_name.otf for the initial file 

and root_name.otfnn on a restart, where nn is the restart number. A file called messag 

is also produced which summarises any error or warnings found during data input and 

initialization. A second summary file containing the same information as the messag file plus 

a summary of the cycle information as the analysis progresses is also produced called 

root_name.log and root_name.lognn on a restart. 

There are also several ASCII time history files that can be written by the code if requested. These 

files have the following names: 

secforc - cross section forces 

rwforc - rigid wall forces 

nodout - nodal point data 

elout - element data 

glstat - global data 

deforc - discrete elements 

matsum - material energies 

ncforc - nodal interface forces 

rcforc - resultant interface forces 

defgeo - smug animator database 

nasbdf - nastran BDF file 

spcforc - SPC reaction forces 

swforc - nodal constraint resultants 

abstat - airbag statistics 

avsflt - ASCII database 

nodfor - nodal force group 

bndout - boundary conditions 

rbdout - rigid body data 

gceout - contact energies 

sleout - interface energies 

Page 3.2


Dump files 

sbtout - seatbelts 

jntforc - joint forces 

tprint - thermal analysis output 

LS-DYNA produces two types of binary dump file that allow analysis to be restarted. The first 

of these is the permanent dump file and a new file is written for each dump. The file name is 

root_name.dpfnn where nn is the dump number. The second type is the auxiliary dump file 

and for this dump the same file is continuously overwritten. The name of the auxiliary dump file 

is root_name.adf. 

Thus for the example analysis given above the following files could be created. 

analysis_ralph_1.dpf01 

analysis_ralph_1.dpf02 

analysis_ralph_1.adf 

On a restart the OASYS_71 shell will rename the chosen dump file to 

analysis_ralph_1.rtf. 

RESTARTING 

What is Restarting? 

Restarting means performing an analysis which continues from a previous analysis. The restart 

can begin from the end of the previous analysis or from part-way through it. It is possible to 

change some of the parameters of the model during a restart. Reasons for doing a restart include: 

! The previous analysis was killed, or exceeded the user-defined CPU limit; the restart then 

completes the analysis. 

! The previous analysis went wrong; to diagnose the error the analysis is restarted from a 

time before the onset of the error, but with more frequent outputs to the results files to 

allow viewing of the development of the error. 

! The previous analysis had some troublesome elements. These can be deleted when 

restarting. 

! A parameter had been wrongly set in the input file but started to have a significant effect 

only after large amounts of CPU had been used. Restarting offers the chance to correct 

the parameter without going back to the beginning. 

Page 3.3


How to Restart an Analysis 

The restarting process is simple. Enter the OASYS command shell, submit the job and opt for 

restart when the menu appears. You will be asked to select which dump file to restart from; the 

available dump files are listed with the analysis times at which they were created. 

Restart Input Files 

A restart input file is needed only if changes are to be made to the model. There are three cases; 

! No restart input file. The analysis will continue unchanged. 

! Short restart input file. 

! Full deck restart input file (see separate notes below). 

The short restart input file must be created by hand; keyword style can be used, and it is 

necessary to create keyword cards only for those items to be changed. Section 28 of the keyword 

manual lists the available keywords. 

An example of a short restart input file is given in Appendix B, Example 8. 

The naming convention for short restart input files is as follows: 

analysis_ralph_1.key - keyword file for original analysis 

analysis_ralph_1.key01 - restart input file for first restart 

analysis_ralph_1.key02 - restart input file for second restart. 

The naming convention is important because it allows the oasys command shell to find the 

correct file. 

The "restart number" is governed by which analysis wrote the restart dump from which the restart 

takes place: e.g. if we are restarting from analysis_ralph_1.dpf03, and this file was 

written by the original analysis, then the restart is by definition the first restart (or restart 1). If 

the first restart writes more restart dump files, including analysis_ralph_1.dpf05, then 

any restart analysis using analysis_ralph_1.dpf05 as a starting point is by definition the 

second restart (or restart 2). 

Effect on Output Files 

Binary output files (.pft, .ctf, .thf and .xtf) are joined seamlessly at the time of the restart. There 

is no way of telling which output states were produced by the original analysis and which by the 

restart analysis. For restarts which began from a point part-way through the original analysis, the 

restart analysis overwrites the original results from that point. 

New ASCII output files are started for each restart: root_name.otf01 and 

root_name.log01 for the first restart, etc. 

Page 3.4


Full Deck Restart 

The Full Deck Restart is a very powerful capability allowing many things to be changed. 

Particularly useful is the ability to redefine contact surfaces, add new contact surfaces, change 

contact parameters, etc. The facility could also be used to replace or add parts, e.g. the new tools 

in a multi-stage sheet metal pressing analysis. 

The full deck restart input file is, as the name suggests, a complete input file. Almost always, 

the input file is a copy of the original input file but with the required changes edited in, and the 

keyword *STRESS_INITIALISATION included. Full deck restarts are used to change 

parameters which cannot be changed with a short restart input file, particularly contact surfaces. 

The full deck restart process is different from the "no input file" or "short restart input file" cases; 

it should be thought of as a new analysis but with stresses, strains, displacements and velocities 

and analysis time carried over from the previous analysis. 

We recommend the following procedure: 

1. Create the full deck restart input file: e.g. copy analysis_ralph_1.key, make the 

required changes, and call the new file analysis_ralph_2.key01. Note that a 

different root file name is chosen, but that the naming convention otherwise follows that 

for short restart input files. 

2. Decide which restart dump file to begin from (e.g analysis_ralph_1.dpf03) then 

copy it as follows: 

cp analysis_ralph_1.dpf03 analysis_ralph_2.rtf 

Note that the new file has the new root name and the extension .rtf. 

3. Submit analysis_ralph_2 in the normal way, ensuring that the restart option is 

selected. Provided that the naming conventions are respected, the oasys shell will find 

the correct files. 

The results files from full deck restart begin at the time of the restart; results generated by the 

original analysis are not included. This is why OASYS recommend use of a different root name 

for the restart analysis. 

Because of the way the full deck restart operates, certain things cannot be changed. These 

include: 

Page 3.5


! Node coordinates 

! Shell, solid, beam or thick shell elements unless a whole PART is deleted. 

! Element topology 

! Element part references 

! Element formulations 

! Material types 

! Anything else which affects storage of element stresses etc, such as element local axis 

systems. 

! Seatbelt retractor, slipring, pretensioner and sensor properties 

! Airbag parameters 

! Rigid body properties (centre of mass, mass inertia tensor) 

! Initial velocities 

! Rigid body extra nodes, merges and anything else that determines which nodes are part 

of which rigid body. 

Other features can in theory be changed, but are likely to cause sudden jumps in stresses when 

the restart occurs; the jumps can in some situations be so violent that the analysis crashes. Such 

features include: 

! Material properties (including properties for spring and belt elements) 

! Section properties 

! Joint stiffness and connectivity 

The following things can be changed: 

! Anything to do with contacts - even introduction of new contact surfaces. All contact 

parameters can be changed. 

! Restraints, constraints and other boundary conditions. 

! Load curves 

! Control parameters (e.g termination time) and output intervals 

It is also possible to add new nodes, elements, parts, etc which were absent from the original 

analysis, and to omit whole parts which were present in the original analysis. The new parts will 

be undeformed at the beginning of the restart analysis, in this case further input is required after 

*STRESS_INITIALISATION. This can be used for multi stage sheet metal pressing 

simulations: the tool models can be replaced at the end of each stage. 

There are some bugs in LS-DYNA affecting full-deck restarts: 

! Spotwelds and tie-break contacts (types 8 & 9) which had failed in the original analysis 

became stuck together again in the restart. 

! The previous history of non-linear contacts (types 9, 20, 21) is lost. The force developed 

on any contacts which was unloading at the time of the restart suddenly jumps to the 

force registered on the loading curve at the current displacement. 

Page 3.6


4.0 KEYWORD INPUT 

The new keyword input database in this version provides a more flexible and logically organised 

database that will hopefully reduce the time required by new users in understanding the input. 

Similar functions are grouped together under the same keyword. For example, under the 

keyword *ELEMENT we not only include solid, beam, and shell elements, but also spring 

elements, discrete dampers, seat belts, and lumped masses. In previous versions these elements 

were specified in separate and disjoint sections of the user's manual. Materials and contact 

algorithms are specified by names and not by type numbers making the data more readable by 

those less familiar with the program. 

The first card should be *KEYWORD. This indicates that the input deck is in keyword format 

and follows this manual. Alternatively KEYWORD may be specified on the execution line. 

LS-DYNA Keyword Manual is alphabetically organized in logical sections of input data. Each 

logical section relates to a particular input. There is a control section for resetting LS-DYNA 

defaults, a material section for defining constitutive constants, an equation of state section, an 

element section where element part identifiers and nodal connectivities are defined, a section for 

defining parts, and so on. Nearly all model data can be input in block form. For example, 

consider the following where two nodal points and shell elements are defined: 

$ 

$ DEFINE TWO NODES 

$ 

*NODE 

10101 x y z 

10201 x y z 

$ 

$ DEFINE TWO SHELL ELEMENTS 

$ 

*ELEMENT_SHELL 

10201 pid n1 n2 n3 n4 

10301 pid n1 n2 n3 n4 

Alternatively, acceptable input could also be of the form: 

$ 

$ DEFINE ONE NODE 

$ 

*NODE 

10101 x y z 

$ 

$ DEFINE ONE SHELL ELEMENT 

$ 

Page 4.1



10201 pid n1 n2 n3 n4 

$ 

$ DEFINE ONE MORE NODE 

$ 

*NODE 

10201 x y z 

$ 

$ DEFINE ONE MORE SHELL ELEMENT 

$ 


10301 pid n1 n2 n3 n4 

A data block begins with a keyword followed by data pertaining to the keyword. The next 

keyword encountered during the reading of the block data defines the end of the block and the 

beginning of a new block. A keyword must be left justified with the "*" contained in column 

one. A dollar sign "$" in column one precedes a comment and causes the input line to be 

ignored. Data blocks are not a requirement for LS-DYNA but they can be used to group nodes 

and elements for user convenience. Multiple blocks can be defined with each keyword if desired 

as shown above. It would be possible to put all nodal points definitions under one keyword 

*NODE, or to define one *NODE keyword prior to each node definition. The entire LS-DYNA 

input is order independent with the exception of the optional keywords *KEYWORD, which 

defines that the input deck uses the new keyword format, and *END, which defines the end of 

input stream. Without the *END termination is assumed to occur when an end-of-file is 

encountered during the reading. 

Figure 4.1 attempts to show the general philosophy of the input organisation and how various 

entities relate to each other. In this figure the data included for the keyword, *ELEMENT, is the 

element identifier, EID, the part identifier, PID, and the nodal points identifiers, the NID's, 

defining the element connectivity: N1, N2, N3, and N4. The nodal point identifiers are defined 

in the *NODE section where each NID should be defined just once. A part defined with the 

*PART keyword has a unique part identifier, PID, a section identifier, SID, a material or 

constitutive model identifier, MID, an equation of state identifier, EOSID, and the hourglass 

control identifier, HGID. The *SECTION keyword defines the section identifier, SID, where a 

section has an element formation specified, a shear factor, SHRF, a numerical integration rule, 

NIP, and so on. The constitutive constants are defined in the *MAT section where constitutive 

data is defined for all element types including solids, beams, shells, thick shells, seat belts, 

springs, and dampers. Equations of state, which are used only with *MAT materials for solid 

elements, are defined in the *EOS section. Since many elements in LS-DYNA use uniformly 

reduced numerical integration, zero energy deformation modes may develop. These modes are 

controlled numerically by either an artificial stiffness or viscosity which resists the formation of 

these undesirable modes. The hourglass control can optionally be user specified using the input 

in the *HOURGLASS section. 

During the keyword input phase where data is read, only limited checking is performed on the 

data since the data must first be counted for the array allocations and then reordered. 

Considerably more checking is done during the second phase where the input data is printed out. 

Page 4.2


Since LS-DYNA has retained the option of reading older non-keyword input files, we print out 

the data into the output file as in previous versions of LS-DYNA. An attempt is made to 

complete the input phase before error terminating if errors are encountered in the input. 

Unfortunately, this is not always possible and the code may terminate with an error message. 

Figure 1Figure 4.1 Organization of the keyword input 

The input data following each keyword can be input in free format. In the case of free format 

input the data is separated by commas, i.e., 

*NODE 

10101,x,y,z 

10201,x,y,z 


10201,pid,n1,n2,n3,n4 

10301,pid,n1,n2,n3,n4 

When using commas, the formats must not be violated. An I8 integer is limited to a maximum 

positive value of 99999999 and larger numbers having more than eight characters are 

unacceptable. Format of the input can change from free to fixed anywhere in the input file. The 

input is case insensitive and keywords can be given in either upper or lower case. THE 

ASTERISKS "*" PRECEDING EACH KEYWORD MUST BE IN COLUMN ONE. 

To provide a better understanding behind the keyword philosophy and how the options work, a 

brief review of some of the more important keywords is given below. 

*AIRBAG 

The geometric definition of airbags and the thermodynamic properties for the airbag inflator 

models can be made in this section. This capability is not necessarily limited to the modelling 

of automotive airbags, but it can also be used for many other applications such as tyres and 

pneumatic dampers. 

Page 4.3


*BOUNDARY 

This section applies to various methods of specifying either fixed or prescribed motion boundary 

conditions. Restraints can be set up as a *BOUNDARY_SPC_NODE section, however, a 

*DEFINE_COORDINATE_SYSTEM is required to define the global coordinate system. For 

compatibility with older versions of LS-DYNA, it is still possible to specify some nodal 

boundary conditions in the *NODE card section. 

*CONSTRAINED 

This applies constraints within the structure between structural parts. For example, nodal rigid 

bodies (*CONSTRAINED_NODAL_RIGID_BODY_OPTION), rivets 

(*CONSTRAINED_RIVET), spotwelds (*CONSTRAINED_SPOTWELD), linear constraints 

(*CONSTRAINED_RIGID_BODIES), adding extra nodes to rigid bodies 

(*CONSTRAINED_EXTRA_NODES_OPTION) and defining rigid body joints 

(*CONSTRAINED_JOINT_OPTION) are all options in this section. 

This section applies constraints within the structure between structural parts. For example, nodal 

rigid bodies, rivets, spotwelds, linear constraints, tying a shell edge to a shell edge with failure, 

merging rigid bodies, adding extra nodes to rigid bodies and defining rigid body joints are all 

options in this section. 

*CONTACT 

This section is divided into three main sections. The *CONTACT section allows the users to 

define a total of 24 different contact types. These contact options are primarily for treating 

contact of deformable to deformable bodies, single surface contact in deformable bodies, 

deformable body to rigid body contact, and tying deformable structures with an option to release 

the tie based on plastic strain. The surface definition for contact is made up of segments on the 

shell or solid element surfaces. 

The *CONTACT_ENTITY section treats contact between a rigid surface, usually defined as an 

analytical surface, and a deformable structure. Applications of this type of contact exist in the 

metal forming area where the punch and die surface geometries can be input as VDA surfaces 

which are treated as rigid. Another application is treating contact between rigid body occupant 

hyper-ellipsoids and deformable structures such as airbags and instrument panels. This option 

is particularly valuable in coupling with the rigid body occupant modelling codes MADYMO and 

CAL3D. 

Each contact definition must start with a *CONTACT_ card. 

The *CONTACT_1D is for modelling rebars in concrete structure. 

*CONTROL 

Options available in the *CONTROL section wither reset default global parameters, such as 

hourglass type, contact penalty scale factor, shell element formulation; or set parameters such as 

termination time. 

Page 4.4


*DAMPING 

Defines damping either globally or by part identifier. 

*DATABASE 

This keyword with a combination of options can be used for controlling the ASCII and binary 

files output by LS-DYNA. This keyword defines the frequencies at which results are written to 

the various databases. 

*DEFINE 

This sections allows the user to define curves for loadings, constitutive behaviours, etc; boxes 

to limit the geometric extent of certain inputs; local coordinate systems; vectors; and orientation 

vectors specific to spring and throughout the input. For example, a coordinate system ID may 

be referenced on a *BOUNDARY_SPC_NODE card for a restraint, and load curves are used on 

the *AIRBAG cards. 

*DEFORMABLE_TO_RIGID 

This section allows the user to switch materials that are defined as deformable to rigid at the start 

of the analysis. This capability provides a cost efficient method for simulating events such as roll 

over events. While the vehicle is rotating the computation cost can be reduced significantly by 

switching deformable materials that are not expected to deform to rigid materials. Just before 

the vehicle comes in contact with ground, the analysis can be stopped and restarted with the 

materials switched back to deformable. 

*ELEMENT 

Solid, shell, thick shell, beam bar(truss), spring, lumped mass and seat belt elements can be set 

up in the input file. The elements used by LS-DYNA are all linear elements (i.e they have no 

mid-side nodes). 

As noted above elements belong to a part and have connectivity with other elements. The part 

has section properties, material properties and hourglass control properties. The connectivity is 

defined by the nodes on the element. Thus the element definition can be seen as a hierarchy as 

follows: 

*ELEMENT,eid,pid,nid1,nid2,nid3,nid4 

*NODE,nid,x,y,z 

... 

*PART,pid sid, mid, eosid,hgid 

*SECTION_SHELL,sid,elform,shrf,nip,propt,qr,icomp 

*MAT_ELASTIC,mid ro,e,pr,da,db 

*EOS,eosid 

*HOURGLASS,hgid 

In most cases the equation of state (*EOS) and hourglass (*HOURGLASS) options can be 

ignored. 

Page 4.5


*END 

This line is optional and flags the end of the input file. 

*EOS 

This section reads the equations-of-state parameters. The equation of state identifier, EOSID, 

points to the equation of state identifer in the *PART card. 

*HOURGLASS 

Defines hourglass and bulk viscosity properties. The identifier, HGID, on the *HOURGLASS 

card refers to HGID on *PART card. 

*INCLUDE 

Keyword input can be read from several files to help manage the data. The file name given after 

the *INCLUDE card is opened and data is then read from that file. If a *END card is found or 

the end of the file is reached, the file is closed and the program continues to read from the 

original file. Several *INCLUDE statements may be in the same file or they may be nested 

through a number of files. 

*INITIAL 

Initial velocity and initial momentum for the structure can be specified in this section. The initial 

velocity specification can be made by *INITIAL_VELOCITY_NODE card or 

*INITIAL_VELOCITY cards. In the case of *INITIAL_VELOCITY_NODE the velocity 

components are specified for individual nodes. Since all the nodes in the system are initialised 

to zero, only the nodes with non-zero velocities need to be specified. The 

*INITIAL_VELOCITY card provides the capability to specify velocities using sets or boxes. 

*INTEGRATION 

In this section the user defined integration rules for beam and shell elements are specified. IRID 

refers to integration rule number IRID on *SECTION_BEAM and *SECTION_SHELL cards 

respectively. Quadrature rules in the *SECTION_SHELL and *SECTION_BEAM cards need 

to be specified as a negative number. The absolute value of the negative number refers to user 

defined integration rule number. Positive rule numbers refer to the built in quadrature rules 

within LS-DYNA. 

*INTERFACE 

Interface definitions are used to define surfaces, nodal lines, and nodal points for which the 

displacement and velocity time histories are saved at some user specified frequency. This data 

may then be used in subsequent analyses as an interface ID in the 

*INTERFACE_LINKING_DISCRETE_NODE as master nodes, in *INTERFACE_ 

Page 4.6


LINKING_SEGMENT as master segments and in *INTERFACE_LINKING_EDGE as the 

master edge for a series of nodes. This capability is especially useful for studying the detailed 

response of a small member in a large structure. For the first analysis, the member of interest 

need only be discretised sufficiently that the displacements and velocities on its boundaries are 

reasonably accurate. After the first analysis is completed, the member can be finely discretised 

in the region bounded by the interfaces. Finally, the second analysis is performed to obtain 

highly detailed information in the local region of interest. When beginning the first analysis, 

specify a name for the interface segment file using the Z=parameter on the LS-DYNA execution 

line. When starting the second analysis, the name of the interface segment file created in the first 

run should be specified using the L=parameter on the LS-DYNA command line. Following the 

above procedure, multiple levels of sub-modelling are easily accommodated. The interface file 

may contain a multitude of interface definitions so that a single run of a full model can provide 

enough interface data for many component analyses. The interface feature represents a powerful 

extension of LS-DYNA's analysis capability. 

*KEYWORD 

Flags LS-DYNA that the input deck is a keyword deck. To have an effect this must be the very 

first card in the input deck. Alternatively, by typing "keyword" on the execute line, keyword 

input formats are assumed and the *KEYWORD is not required. This keyword can also be used 

to specify the amount of memory, in words, that the analysis is to use by adding the required 

amount to the input line ,e.g *KEYWORD 5000000. 

*LOAD 

This section provides various methods of loading the structure with concentrated point loads, 

distributed pressures, body force loads, and variety of thermal loadings. 

*MAT 

This section allows the definition of constitutive constants for all material models available in 

LS-DYNA including springs, dampers, and seat belts. The material identifier, MID, points to 

the MID on the *PART card. 

*NODE 

Define nodal point identifiers and their coordinates. 

*PART 

This keyword serves two purposes. 

1. Relates part ID to *SECTION, *MAT, *EOS and *HOURGLASS sections. 

2. Optionally, in the case of a rigid material, rigid body inertia properties and initial 

conditions can be specified. Deformable material repositioning data can also be specified 

in this section if the reposition option is invoked on the *PART card, i.e., 

*PART_REPOSITION. 

Page 4.7


*RIGIDWALL 

Rigid wall definitions have been divided into two separate sections _PLANAR and 

_GEOMETRIC. Planar walls can be either stationary or moving in translational motion with 

mass and initial velocity. The planar wall can be either finite or infinite. Geometric walls can 

be planar as well as have the geometric shapes such as rectangular prism, cylindrical prism and 

spherical. By default these walls are stationary unless the option MOTION is invoked for either 

prescribed translational velocity or displacement. Unlike the planar walls, the motion of the wall 

is governed by the load curve. Multiple geometric walls can be defined to model combinations 

of geometric shapes available. For example, a wall defined with the _CYLINDER option can 

be combined with two walls defined with the _SPHERICAL option to model hemispherical 

surface caps on the two ends of a cylinder. Contact entities are also analytical surfaces but have 

the significant advantage that the option can be updated based upon the equations of rigid body 

mechanics or prescribed with six full degrees-of-freedom. 

*SET 

A concept of grouping nodes, elements, parts etc. in sets is employed throughout the LS-DYNA 

input deck. Sets of data entities can be used for output. Slave nodes used in contact definitions, 

slaves segment sets, master segment sets, pressure segment sets and so on can also be defined. 

The keyword, *SET, can be defined in two ways. 

1. Option _LIST requires a list of entities, eight entities per card and define as many cards 

as needed to define all the entities. 

2. Option _COLUMN where applicable requires an input of one entity per line along with 

up to four attribute values which are needed to specify for example failure criterion input 

that is needed for *CONTACT_CONSTRAINT_NODES_TO_SURFACE. 

*USER_INTERFACE 

This section provides a method to provide user control of some aspects of the contact algorithms 

including friction coefficients via user defined subroutines. 

*TITLE 

In this section a title for the analysis is defined. 

RESTART 

This section of the input is intended to allow the user to restart the simulation by providing a 

restart file and optionally a restart input defining changes to the model such deleting contacts, 

materials, elements, switching materials from rigid to deformable, deformable to rigid, etc. 

*RIGID_TO_DEFORMABLE 

This section switches rigid materials back to deformable in a restart to continue the event of a 

vehicle impacting the ground which may have been modelled with a rigid wall. 

Page 4.8


*STRESS_INITIALIZATION (Full Deck Restart) 

This is an option available for restart runs. In some cases there may be a need for the user to add 

contacts, elements, etc., which are not available options for restart runs. A full input containing 

the additions is needed if this option is invoked upon restart. 

Users new to the keyword method of input may find difficulties in locating the correct keyword 

to use. The following table is an aid to locating the correct keyword for the most commonly used 

options. 

Topic Component Keyword 

Geometry Nodes 

Elements 

Discrete Elements 

Materials Part (which is composed 

of Material and 

Section, equation of 

state and hourglass 

data) 

Material 

Sections 

Discrete sections 

Equation of state 

Hourglass 

*NODE 

*ELEMENT_BEAM 


*ELEMENT_SOLID 

*ELEMENT_TSHELL 

*ELEMENT_DISCRETE 

*ELEMENT_MASS 

*ELEMENT_SEATBELT_Option 

*PART 

*MAT_Option 

*SECTION_BEAM 

*SECTION_SHELL 

*SECTION_SOLID 

*SECTION_TSHELL 

*SECTION_DISCRETE 

*SECTION_SEATBELT 

*EOS_Option 

*CONTROL_HOURGLASS 

*HOURGLASS 

Page 4.9


Rigid Bodies Defining body 

Contacts and 

Rigidwalls 

Boundary 

Conditions & 

Loadings 

Constraints and 

spot welds 

Extra nodes 

Merged bodies 

Nodal rigid bodies 

Defaults for contacts 

Definition of contacts 

Definition of rigidwalls 

Restraints 

Gravity (body) load 

Point load 

Pressure load 

Thermal load 

Load curves 

Constrained nodes 

Welds 

Rivet 

Output Control Defaults 

ASCII time history files 

Binary plot, time history and 

restart files 

Items in time history blocks 

Nodes for nodal reaction 

output 

Termination Termination time 

Termination cycle 

CPU termination 

Degree of freedom 

*PART 

*MAT_RIGID 

*PART_INERTIA 

*CONSTRAINED_EXTRA_NODES_Option 

*CONSTRAINED_RIGID_BODIES 

*CONSTRAINED_NODAL_RIGID_BODY_Option 

*CONTROL_CONTACT 

*CONTACT_Option 

*RIGIDWALL_Option 

*NODE 

*BOUNDARY_SPC_Option 

*LOAD_BODY_Option 

*LOAD_NODE_Option 

*LOAD_SEGMENT_Option 

*LOAD_SHELL_Option 

*LOAD_THERMAL_Option 

*DEFINE_CURVE 

*CONSTRAINED_NODE_SET 

*CONSTRAINED_GENERALIZED_ WELD_Option 

*CONSTRAINED_SPOT_WELD 

*CONSTRAINED_RIVET 

*CONTROL_OUTPUT 

*DATABASE_Option 

*DATABASE_BINARY_Option 

*DATABASE_HISTORY_Option 

*DATABASE_NODAL_FORCE_GROUP 

*CONTROL_TERMINATION 


*CONTROL_CPU or via Oasys_71 shell 

*TERMINATION_NODE 

Page 4.10


5.0 UNITS 

There is no way of telling LS-DYNA what units the model uses so units must be compatible. 

One way of testing whether a set of units is compatible is to check that: 

1 (force unit) = 1 (mass unit) x 1 (acceleration unit) 

and that 1 (acceleration unit) = 1 (length unit) 

[1 (time unit)]² 

Examples of sets of compatible units are: 

(a) (b) © 

Length unit metre millimetre millimetre 

Time unit second second millisecond 

Mass unit kilogramme tonne kilogramme 

Force unit Newton Newton kiloNewton 

Young's Modulus of Steel 210E9 210E3 210 

Density of Steel 7.85E3 7.85E-9 7.85E-6 

Yield stress of Mild Steel 200E6 200 0.200 

Acceleration due to gravity 9.81 9.81E3 9.81E-3 

Velocity equivalent to 30mph 13.4 13.4E3 13.4 

Page 5.1


Page 5.2


6.0 MATERIAL MODELS 

LS-DYNA includes over 100 material models and is able to represent a wide range of material 

behaviours. Section 16 of the theory manual covers the equations used by the various models. 

In the User Manual, materials appear in order of their type number rather than alphabetically (e.g. 

the first material listed is MAT_ELASTIC, type 1). The type number is given on the keyword 

page for each material. 

PLASTICITY MODELS 

The basic elastoplastic material model (MAT_PLASTIC_KINEMATIC, type 3) has a bilinear 

stress-strain curve. The user defines the yield stress and hardening modulus. There is a choice 

of isotropic or kinematic hardening (or behaviour between these extremes); this refers to how 

work-hardening affects the yield stress when the loading is reversed, e.g. what is the yield stress 

for compressive loading following yield in tension. 

Material type 12 (MAT_ISOTROPIC_ELASTIC_PLASTIC) is a simplified version giving 

isotropic hardening only. For shell elements a one step radial return is used; volume is not 

conserved during plastic flow and this can cause serious errors in some situations. Therefore, 

material type 12 is not recommended for shell elements. For both brick and shell elements, 

computing effort is reduced compared with Material type 3. 

Variants on the bilinear theme include material type 4 

(MAT_ELASTIC_PLASTIC_THERMAL), which allows the properties to vary with 

temperature, and type 17 (MAT_ORIENTED_CRACK), which includes fracture at a pre-defined 

tensile stress. Hardening properties may exist in terms of an "n" value. In this case, material type 

18 (MAT_POWER_LAW_PLASTICITY) can be used. 

If tensile test data is available, the stress-strain points can be entered for use with material type 

24 (MAT_PIECEWISE_LINEAR_PLASTICITY). This is generally recommended for 

crashworthiness analysis. When using tensile test data to derive the input stress and strain values, 

first convert to true stress and true strain ( c true = c nominal[1+ … nominal], … true = ln[1+ … nominal] ). 

Beyond the Ultimate Tensile Strength the experimental curve is hard to interpret because all the 

deformation is concentrated in the neck region; it is recommended that the input curve be made 

flatter beyond UTS than the experimental curve to allow for the uncertainties. The failure strain 

should generally be set based on reduction in cross-sectional area when the tensile test specimen 

fails (this is significantly greater than the apparent "true strain" in the specimen as a whole, due 

to local effects in the neck). 

Page 6.1


The formula is: 

failure strain = ln (original area) 

area at failure 

Resultant plasticity (type 28) can be used with Shell or Belytschko-Schwer beam elements to 

bypass the normal solution method which calculates stresses at each integration point in the 

cross-section. This is computationally cheaper but can be inaccurate in some situations. 

Strain rate sensitivity can be included in many of the material types e.g. types 3, 18 and 24 allow 

input of Cowper Symonds rate effect parameters. Typical values for mild steel are c = 1300s -1 

and p = 5. There is generally less rate effect in high strength steels. If experimental data is 

available, use the curve LCSR in material type 24 to define how the rate effect varies with strain 

rate the viscoplastic option gives much smoother response but at cost of higher CPU usage. 

CONCRETE 

Concrete can be represented using material type 78 (MAT_SOIL_CONCRETE), which includes 

both volumetric crushing and strain softening in shear (to simulate cracking). 

RUBBER 

Material type 27 (MAT_MOONEY_RIVLIN_RUBBER) is generally reliable. Others available 

include types 31, 77, 7 and 6. Of these, 7 is not recommended. For low strain applications type 

6 is recommended. 

FOAM 

Material types 38 (MAT_BLATZ_KO_FOAM), 53 (CLOSED_CELL_FOAM), 57 

(MAT_LOW_DENSITY_FOAM), 62 (MAT_VISCOUS_FOAM), 63 

(MAT_CRUSHABLE_FOAM), 75 (MAT_BILKHU_DUBOIS_FOAM) and 83 (FU-CHANG- 

FOAM) are all written specifically for foams. It is also possible to model foams using material 

types 5 (MAT_SOIL_AND_FOAM) and 26 (MAT_HONEYCOMB). Oasys recommend the 

following: 

! For materials which show permanent crush (e.g. expanded polystyrene, ureaformaldehyde 

foam, etc.), use material type 63. A stress-strain load curve is defined, and 

unloading is elastic. 

! For materials which show hysteretic stress-strain behaviour but which recover to close 

to the original shape, use material type 57. With HU set to 0.01 and BETA set to 0.0, the 

amount of hysteresis depends on SHAPE. SHAPE = 10.0 gives high hysteresis (most of 

the energy is absorbed) while SHAPE = 0.1 gives negligible hysteresis. 

Page 6.2


! If the material is orthotropic (different crush strength in different directions), and the 

orthotropicity is important to the model, use material type 26. The input is more complex 

than for materials 57 and 63. 

It is often worth using fully integrated brick elements to represent foams; these are better able to 

withstand localised loading without causing hourglass deformations in neighbouring elements. 

Tetrahedral elements using ELFORM = 10 are especially stable. 

ELEMENT FAILURE 

Many material models give the option of having elements fail (e.g. type 24). At failure the 

elements cease to carry load, and any contact segments upon them are removed. Nodes can then 

fall through the resulting holes in contact surfaces. The list of failed elements is written to the 

complete state file where it can be detected by OASYS D3PLOT and OASYS D/CODE, and thus 

the failed elements can be removed during post-processing. (D3PLOT automatically blanks out 

failed elements). 

The *MAT_ADD_EROSION facility allows the user to set up a failure criterion for solid 

elements of any material type, based on stress or strain data such as pressure, principal stress, or 

principal strain. This is useful for castings, plastics, etc where the more usual, plastic strainbased 

failure criteria are inappropriate. 

Page 6.3


Page 6.4


7.0 ELEMENTS 

The elements shown in Figures 7.1 and 7.2 are presently available. 

Figure 7.1 Elements in OASYS DYNA3D 

Figure 7.2 Discrete Elements 

Element formulations are described in the Theory Manual, Sections 3 to 13. 

Page 7.1


SOLIDS 

The 8-node solid element by default uses one point integration plus viscous hourglass control. 

Fully integrated brick elements are also available (see SECTION_SOLID and Section 3.3 of the 

Theory Manual); these perform better where element distortions are large but are about four 

times more costly. No hourglass control is needed as there are no zero-energy modes. Wedges 

and tetrahedra are simply degenerate bricks (i.e some of the nodes are repeated); they cause 

problems in some situations and are best avoided. 

SHELLS 

All shell elements include membrane, bending and shear deformation. The default Belytschko- 

Tsay formulation is the most economical and should be used unless features particular to other 

formulations are required e.g.: 

- Hughes Liu : can offset the mid-plane of the element away from the nodes. 

- S/R co-rotational Hughes-Liu : fully integrated, so hourglass deformations do not occur 

(but much more costly). 

- Belytschko-Tsay membrane (and fully integrated membrane): appropriate for fabrics etc. 

where bending stiffness is negligible. 

As degenerate quadrilateral shell elements are prone to lock under transverse shear, triangular 

shell elements have now been implemented, based on work by Belytschko and co-workers [35- 

37]. Triangular shells can be mixed with quadrilateral shells within the same material property 

set, provided that the element sorting flag (ITRIST on CONTROL_SHELL) is set to 1. 

Three-dimensional plane stress constitutive subroutines are implemented for the shell elements 

which update the stress tensor such that the stress component normal to the shell mid surface is 

zero. The integration points are stacked vertically at the centroid of the element, as shown in 

Figure 7.3. 

Figure 7.3 Integration Points 

Page 7.2


Through-thickness directions at each node are initially normal to the element surface but rotate 

with the nodes. Strains are linear through the thickness. Two integration points are sufficient 

for linear elastic material, while more points are required for nonlinear material. Stress output 

gives stresses at the outermost integration points, not at the surfaces (despite the nomenclature 

of post-processors, which refer to top and bottom surfaces), so care is needed in interpretation 

of results. For elastic materials, stresses can be extrapolated to the surfaces. For nonlinear 

materials the usual policy is to choose four or five integration points through the thickness and 

to ignore the error (i.e. the difference in stress between the surface and the outermost integration 

point). The location of the outermost integration points are given in the following table: 

THICK SHELLS 

________________________________________________ 

Mid Plane 0 

(2 points .5774 ) 

Outermost (3 points .7746 ) 

Point (4 points .8611 ) 

(5 points .9062 ) 

Outer Surface 1.0 

________________________________________________ 

The thick shell element is an eight node brick-shell. The through-thickness direction and 

thickness at each corner of the thick shell is defined by the relative position of the two nodes; 

rotational degrees of freedom are ignored. Through-thickness deformation is resisted by a 

penalty stiffness, although through-thickness stress is taken as zero in the constitutive models. 

This means that contact can occur on both faces of the shell, but the compressive stresses 

produced by this will not "extrude" the element and may not be reported by post-processing. As 

the through-thickness direction of the thick shell element is treated differently to the in-plane 

directions it is vital that the topology of the element be defined correctly. The thick shell cannot 

be degenerated to a wedge or tetrahedron. 

BEAMS 

The Hughes-Liu beam is a conventionally integrated element able to model rectangular or 

circular cross-sections using an array of integration points at the mid-span of the element. 

Alternatively, the user may specify a cross-section integration rule to model arbitrary crosssections. 

The beam effectively generates a constant moment along its length, so, as with the 

brick and shell elements, meshes need to be reasonably fine to achieve adequate accuracy. 

Because of the location of the integration points yielding is detected only at the element centre. 

Therefore a model cantilever beam will yield at slightly too high a force because the fully plastic 

moment must be developed at the centre of the encastré element rather than at the root. 

Page 7.3


The Belytschko-Schwer beam is explicitly formulated and generates a moment which varies 

linearly along the length of the beam. The elements have the "correct" elastic stiffnesses and 

detect yielding at their ends. For example, a cantilever loaded statically at its tip can be 

represented accurately in both elastic and plastic regimes using a single element. If Material type 

29 is used, the following non-linear behaviour is catered for: 

a) Axial crushing, where the crush force-strain relationship is supplied by the user. 

b) Rotation at plastic hinges, where the moment-rotation relationship is supplied by the user. 

The hinges can form at either end of each element. 

As with the Hughes-Liu beam, the mass is lumped onto the nodes, so finer meshes may be 

required for dynamic problems where a correct mass distribution is important. 

The Truss element is similar to the Belytschko-Schwer beam but carries axial loads only. 

The Discrete Beam is similar to a spring element, in that relationships between force and 

deformation are input directly by the user. 

RIGID BODIES 

All element classes can be declared as rigid bodies. Rigid bodies are covered in detail in Section 

8. 

DISCRETE ELEMENTS 

Discrete mass, spring and damper elements are also available. 

Spring elements generate a force which depends on displacement (i.e. change of length of the 

element; length is defined as the dot product of the line from node 1 to node 2 with the element 

axis direction. Usually this means the change of absolute length between the nodes of the 

element irrespective of any rotation of the element.). The force is applied along the element axis. 

For example, a positive force (tension) acts along the positive axis direction on node 1 and along 

the negative axis direction on node 2. 

By default, the element axis lies along the line from node 1 to node 2. When the element rotates, 

the line of action of the force also rotates. Alternatively, the user may select a fixed axis or a 

fixed plane onto which the element will be projected to obtain the axis. A further option is to 

define a moving axis defined by any two nodes. These options are selected using Orientation 

Vectors. It should be noted that the sign of the displacement depends on the direction of the axis; 

if the dot product of the selected axis and the line from node 1 to node 2 is negative, elongation 

of the spring will result in compressive displacements. That is, the definition of tension and 

compression will become reversed. This does not matter if the force-displacement relationship 

is the same in tension and compression. 

Page 7.4


The default axis option can be dangerous if the two nodes of the element pass through each other; 

the element axis then turns through 180 degrees and the forces are reversed, leading to sudden 

large deformations. If this situation is likely, or if the nodes are initially coincident, a fixed axis 

should be used. 

Damper elements are treated as a subset of spring elements: spring material types 2 and 5 are 

linear and nonlinear dampers respectively. 

Rotational springs and dampers are also available. These are selected by setting a flag in the 

spring material input. The rest of the input is the same as for translational springs; the given 

force-displacement relationship will be treated as moment-rotation (rotation in radians), and the 

moments are applied about the element axis (positive clockwise). The default axis type should 

not be used. Instead, a fixed axis can be selected, or if the spring is attached to a rotating body, 

two nodes in that body can be selected to define the axis. 

Rotational springs affect only the rotational degrees of freedom of their nodes - they do not pin 

the nodes together. 

Spring and damper element forces and extension are automatically sent to the XTF file for 

plotting by T/HIS, provided that the XTF file is written i.e. a *DATABASE_BINARY_XTFILE 

card is present). The elements can also be viewed in D3PLOT, again provided that the XTF file 

is written. 

An alternative option for viewing spring and damper elements is available: non-structural beam 

elements can be created automatically, coincident with each spring/damper element. These can 

be viewed in LS-TAURUS, etc. To activate this option, set NOBEAM on 

*DATABASE_BINARY_D3PLOT to zero. Note that the non-structural beam elements appear 

by default unless NOBEAM is set to 1. The beams have the same label as the parent spring 

element; consequently no structural beam element must have the same label as any spring 

element if the non-structural beams are being used. 

SEAT BELT ELEMENTS 

This version of LS-DYNA introduces a number of special elements to allow seat belts to be 

modelled. These elements include seat belts, slip rings, retractors, pretensioner and sensors. 

These element are described in Section 13.9 to 13.14 of the Theory Manual. 

MASS DISTRIBUTION 

The mass of each solid, shell, beam and thick shell element is distributed equally onto the nodes 

of the element. In the case of shell and beam elements a rotational inertia is also added to each 

node; a single value is used, so that the effect is to distribute the mass spherically around the 

node. 

Page 7.5


Page 7.6


8.0 RIGID BODIES 

DEFINITION 

Rigid bodies are defined by declaring a part which references a material of type 20 

(MAT_RIGID). All elements of that part number are then considered part of the same rigid 

body; they do not have to be linked by mesh connectivity. To represent more than one 

independent rigid body in a model, a part with material type 20 should be defined for each body: 

it is the part number which distinguishes one body from another. 

The input includes Young's modulus and Poisson's Ratio; these are required so that the stiffness 

of contact surfaces can be calculated. It is recommended that properties similar to those of the 

deformable materials be used, unless the rigid body elements are much larger than the deformable 

elements. In this case, scale the Young's modulus down so that the product of element length and 

Young's modulus is similar for the rigid and deformable elements. 

HOW THEY WORK 

The mass, centre of mass and inertia properties of each rigid body are calculated on initialisation 

from the volume and density of the elements. Thereafter, the forces and moments acting on the 

body are summed from the nodal forces and moments, at each timestep. The motion of the body 

is calculated and this is then imposed on its nodes. Because of this, other features which also 

work by imposing motion on nodes should not be applied to nodes on rigid bodies, e.g. 

constraints, tied interfaces, etc. It is also an error if two rigid bodies share a common node. 

MASS AND INERTIA PROPERTIES 

It is possible to override the automatically calculated mass, centre of mass and inertia for any 

rigid body and also to define an initial velocity. This is done using *PART_INERTIA instead 

of simply *PART. 

Inertia values are defined as follows: 

I xx = Pm[(y-y a)² + (z-z a)²] 

I xy = -Pm[(x-x a)(y-y a)] 

I xz = -Pm[(x-x a)(z-z a)] 

I yy = Pm[(x-x a)² + (z-z a)²] 

I yz = -Pm[(y-y a)(z-z a)] 

I zz = Pm[(x-x a)² + (y-y a)²] 

(x a, y a, z a) = centre of mass. 

If non-zero values are entered for the off-diagonal inertia terms (I xy, etc), it is important that these 

are consistent with the diagonal terms (I xx, etc). If this is not done, the principal inertias can 

Page 8.1


become negative. The symptom of this is that the body begins to rotate, often slowly at first, but 

at growing speed until the analysis crashes. 

RESTRAINTS 

Restraints on rigid bodies are defined on the material input, card 2. These allow translations of 

the centre of mass, and rotations about axes through the centre of mass, to be clamped. Two 

methods are available: 

- Restraints in global axes (CMO = +1.0) 

- Restraints in local axes using SPC restraint codes (CMO = -1.0) 

While it is also possible to restrain rigid bodies by restraining at least 3 non-collinear nodes, this 

is not recommended. If restraints are defined on the material cards, these override any nodal 

restraints. The restraint condition of each rigid body is printed in the .OTF file during the input 

phase. 

It is not possible to pin' a rigid body simply by restraining one node; the motion imposed by the 

rigid body will override the restraints. A pinned condition can be achieved by declaring the 

centre of mass to be at the pin location and restraining all translational degrees of freedom of the 

body. Alternatively, a spherical joint to a fully restrained rigid body can be created. 

It is recommended to check the restrain conditions of rigid bodies in the OFT file: Search for “r 

i g i d b o d y c o n s t r a i n t s” 

JOINTS 

Joints can be used to link two rigid bodies together (see *CONSTRAINED_JOINT). Spherical, 

revolute and cylindrical types are recommended. All the joints work by a penalty method, i.e. 

any relative displacement in a direction which the joint restrains is resisted by a force 

proportional to the displacement. The stiffness of the joints is calculated automatically, and is 

the maximum value which will not give rise to instability. If desired, the user can reduce the 

stiffness by entering a relative penalty stiffness less than 1.0 on the joint cards. 

Spherical joints act as a pin, preventing relative translation but allowing rotation. Revolute joints 

act as a pair of pins, allowing only relative rotational about the axis through the pins. Cylindrical 

joints allow relative translation along, and rotation about, an axis which is fixed in one of the two 

rigid bodies. 

EXTRA NODES 

Extra nodes may be added to a rigid body using *CONSTRAINED_EXTRA_NODES. The 

effect is the same as if the nodes were attached to elements of the body. 

Page 8.2


RIGID BODY MERGE 

Two rigid bodies can be merged together so that they act as a single rigid body. The input (see 

*CONSTRAINED_RIGID_BODIES) consists of two part numbers, both of which must be rigid 

(i.e. reference type 20 materials). The second body is absorbed into the first, and any subsequent 

references to the second body become meaningless. Thus if three rigid bodies are to be merged 

together (say A, B and C) the correct procedure is to merge A with B, then A with C. A will then 

include all the elements and nodes of B and C. If inertia properties are to be defined for the 

merged body, these should reference material A. 

Rigid body merges can be used to avoid the error which arises if two bodies share common 

nodes. By merging the two bodies the nodes then belong only to the first body. 

DEFINED VELOCITIES 

The motion of a rigid body can be prescribed by using Displacement or Velocity Boundary 

Conditions (see *BOUNDARY_PRESCRIBED_MOTION_RIGID). These should be applied 

to the body as a whole, not to the individual nodes (i.e. don't use 

*BOUNDARY_PRESCRIBED_MOTION_NODE for nodes belonging to rigid bodies). 

Rotational velocities are applied at the centre of mass. 

OUTPUT 

The elements which form a rigid body can be plotted in the normal way using I-DEAS, CAEDS, 

NISA DISPLAY, PATRAN, OASYS D3PLOT, etc. Stresses and strains in the elements and 

shell thicknesses appear as zero. If the contact stress output file (.CTF) is used (see Section 8) 

then contact stresses on the rigid bodies can be plotted using OASYS D3PLOT. 

Time-histories of nodal displacements, velocities and accelerations, and the kinetic energy of 

each rigid body, can be plotted using OASYS T/HIS. 

Page 8.3


Page 8.4


9.0 CONTACT SURFACES 

CONTACT SURFACE DEFINITION 

Contact surfaces in LS-DYNA allow the user to represent a wide range of types of interaction 

between components in a model. This section is intended as an introductory guide; see Theory 

Manual, Section 23 for further details. 

Contact surfaces are defined using sets, which can contain "segments" (3- or 4-node element 

faces), nodes, shell elements, or parts. If the set contains parts, all the elements made of those 

parts are included in the contact. Optionally, a box can also be defined: in this case, only the 

elements in the box are included in the contact. Generally, two sets are defined - the slave and 

the master. Any entity in the slave set can contact any entity in the master set and vice versa. 

However, with the single surface types, only one set is defined (the slave) and any entities in the 

set can contact any other entity in the same set. 

TYPES OF CONTACT SURFACE 

Contact surfaces are specified by their type names in the keyword input deck. For historical 

reasons, the types are sometimes referred to by type “numbers”. Both ways of specifying contact 

types are listed below. Some contact types have variants, for which the type number is preceded 

by a letter. 

The most commonly used contact types are: 

Type a3 *CONTACT_AUTOMATIC_SURFACE_TO_SURFACE 

Type a5 *CONTACT_AUTOMATIC_NODES_TO_SURFACE 

Type 13 *CONTACT_AUTOMATIC_SINGLE_SURFACE 

Users may encounter the following types: 

TIED: 

Type 2: *CONTACT_TIED_SURFACE_TO_SURFACE 

Type o2: *CONTACT_TIED_SURFACE_TO_SURFACE_OFFSET 

Tied contact surfaces "glue" the slaves to the masters. The slave and master segments should 

initially be coplanar. During initialisation, for each slave node, the contacted master segment is 

found and the isoparametric position of the slave node within that segment is calculated. 

Thereafter, the slave node is forced to maintain its isoparametric position within the master 

segment. The effect is that the master segments can deform and the slave nodes are forced to 

follow that deformation. Equilibrium is maintained and forces are transmitted correctly across 

the tied surface, but shock waves may be partially reflected. 

Of the two surfaces, the coarser one should be defined as the master. Only translational degrees 

Page 9.1


of freedom are affected - slave nodes are effectively "pinned" to the master surface. Type 2 

surfaces work by a kinematic constraint method: see the "Errors and Warnings" section below. 

Any slave nodes that are initially far from the master segments will not be constrained. Slave 

nodes that are near a master segment but are slightly offset will be constrained, but the offset can 

lead to rotational constraints that cause erroneous results. 

Tied surfaces involving nodes that are constrained in other ways or are offset from the master 

segments should be of type o2. This type uses a penalty method that does not require nodes to 

be unconstrained or to lie exactly on master segments. 

SLIDING WITH VOIDS 

Type 3: *CONTACT_SURFACE_TO_SURFACE 

Type a3: *CONTACT_AUTOMATIC_SURFACE_TO_SURFACE 

Type m3: *CONTACT_FORMING_SURFACE_TO_SURFACE 

This type of surface is widely used to represent contact between components in a model. 

Compression can be carried but not tension - the two components can separate. Sliding can be 

resisted by friction. 

On initialisation, the master node nearest to each slave node is found, and the master segments 

attached to that node will be the first to be checked for contact. The process is repeated for the 

master nodes and slave segments. Thereafter, sliding may mean that nodes move from one 

segment to another. In type 3, this process is tracked using mesh connectivity: instead of 

checking all segments for contact, only those segments attached to nodes of the previously 

contacted segment will be checked. As a consequence, contact cannot be tracked across free 

edges. Examples are given in the "Errors and Warnings" section below. Note that the search 

method changes to “bucket sort” (see below) if SHLTHK on *CONTROL_CONTACT is nonzero 

- see below. If type a3 (automatic surface to surface) is specified, the bucket sort method is 

always used. 

Once the contacted segments have been found for each node, the amount of penetration of the 

slave node into the master segment is calculated and resisted by a penalty stiffness. The process 

is repeated for the master nodes and slave segments. The stiffness calculation is described below. 

Because the treatment is symmetric, it does not matter which surface is defined as the master and 

which as the slave. It is possible for nodes to be part of several different contact surfaces. 

Initial gaps between the slaves and masters are allowed but not necessary. If any nodes are 

initially penetrating they will be moved back to the surface and a message will be printed in the 

.OTF and .LOG files. This check can be omitted by setting the flag on Control Card 9, Column 

25, to 1. In this case initial penetrations will lead to contact forces being developed on the first 

timestep. 

Type m3 surfaces are for use in metalforming simulation. They allow negative surface offsets to 

be specified so that the same mesh geometry can be used for both the punch and the die. If the 

Page 9.2


mesh is continuous, a very high bucket sort interval can be specified so that only one bucket sort 

is performed, at the beginning of the analysis. This can give significant improvements to 

computational efficiency. 

SINGLE SURFACE 

Type 13: *CONTACT_AUTOMATIC_SINGLE_SURFACE 

Type 26: *CONTACT_AUTOMATIC_GENERAL 

These are similar to the “sliding with voids” contact types, except that the slave nodes contact 

other slave segments. There are no masters. Single surface contact is used where a more general 

contact capability is required, i.e. there is no need to define what contacts what. 

Likely candidate segments for contact by each node are identified by a bucket sort. The effect of 

this is that meshes do not have to be continuous. 

Type 26 is a more robust, but slower, version of type 13. In type 26 contact, nodes can penetrate 

up to 400 times the segment thickness without being set free. Shell edge-to-edge and beam-tobeam 

contact is also considered. Type 26 contacts are processed at approximately half the speed 

of type 13 contacts. 

NODES TO SURFACE 

Type 5: *CONTACT_NODES_TO_SURFACE 

Type a5: *CONTACT_AUTOMATIC_NODES_TO_SURFACE 

Type m5: *CONTACT_FORMING_NODES_TO_SURFACE 

Types 5, a5 and m5 surfaces are the same as types 3, a3 and m3 except that: 

- The slave side is defined by individual nodes (or parts) instead of segments. 

- The treatment is not symmetric: only contact of slave nodes with master segments is 

considered. 

If the mesh of one side is significantly coarser than the other, then the coarser side should be the 

master (with segments defined). 

Type 5 surfaces are computationally cheap and are recommended for many applications, 

particularly where one side is on a rigid body or consists of beam or spring elements and hence 

segments cannot be defined. 

TIED NODES TO SURFACE 

Page 9.3


Type 6: *CONTACT_TIED_NODES_TO_SURFACE 

Type o6: *CONTACT_TIED_NODES_TO_SURFACE_OFFSET 

These are the same as types 2 and o2 except that the slave side is defined by individual nodes 

instead of segments. 

SHELL EDGE TIED TO SHELL SURFACE 

Type 7: *CONTACT_TIED_SHELL_EDGE_TO_SURFACE 

Type o7: *CONTACT_TIED_SHELL_EDGE_TO_SURFACE_OFFSET 

These are the same as types 6 and o6 except that rotational degrees of freedom are also tied 

together, allowing moments to be transferred. 

NODES SPOTWELDED TO SURFACE 

Type 8: *CONTACT_TIEBREAK_NODES_TO_SURFACE 

Slave nodes are tied to the masters until a failure criterion is reached. Thereafter they can slide 

on or separate from the masters as in a type 5 contact surface. This type of surface can be used 

to represent spot-welded or bolted connections. 

Before failure, pinning is achieved using penalty stiffness, not kinematic constraint, so the 

warnings applying to tied interfaces do not apply to type 8. 

TIEBREAK 

Type 9: *CONTACT_TIEBREAK_SURFACE_TO_SURFACE 

This is similar to type 8 except that failure is based on stress rather than force at individual nodes. 

It can be used to model fracture or rupture of a component where the failure plane is known in 

advance, for example bolts in the lid of a transport container. 

ONE WAY SLIDING WITH VOIDS 

Type 10: *CONTACT_ONE_WAY_SURFACE_TO_SURFACE 

Type a10: *CONTACT_AUTOMATIC_ONE_WAY_SURFACE_TO_SURFACE 

Type m10: *CONTACT_FORMING_ONE_WAY_SURFACE_TO_SURFACE 

These are identical to types 5, a5 and m5 except that the slave surface is defined using segments 

(or parts) instead of nodes. 

Page 9.4


ERODING CONTACT 

Type 14: *CONTACT_ERODING_SURFACE_TO_SURFACE 

Type 15: *CONTACT_ERODING_SINGLE_SURFACE 

Type 16: *CONTACT_ERODING_NODES_TO_SURFACE 

These are used instead of types 3, 13 and 5 respectively where solid elements may fail. The 

purpose of these is to allow contact to occur with the remaining elements, after the elements 

originally forming the surface have failed. 

CONSTRAINT CONTACT 

Type 17: *CONTACT_CONSTRAINT_SURFACE_TO_SURFACE 

Type 18: *CONTACT_CONSTRAINT_NODES_TO_SURFACE 

Types 17 and 18 are similar to types 3 and 5, respectively, except that the penetrating slaves and 

masters are constrained to move together, using conservation of momentum to determine the 

combined velocity. This method eliminates contact penetrations and is useful for high pressure 

or high-speed impacts where penalty methods would generate unacceptably high penetrations. 

However, they cannot be used with nodes that are constrained in other ways, and are prone to 

instability problems if artificial penetrations occur (see later). 

NONLINEAR CONTACTS 

Type 19: *CONTACT_TWO_WAY_RIGID_BODY_TO_RIGID_BODY 

Type 20: *CONTACT_RIGID_NODES_TO_RIGID_BODY 

Type 21: *CONTACT_RIGID_BODY_ONE_WAY_TO_RIGID_BODY 

Contact types 19, 20 and 21 are similar to types 3, 5 and 10 respectively, except that instead of 

a linear stiffness to resist penetration, the user defines a force-deflection curve. They are 

intended to allow inclusion of energy-absorbing compliance without the need for modelling 

deformable elements. More details are given under "Contact Surface Stiffness" - see below. 

GEOMETRIC CONTACTS 

It is possible to model contact between an arbitrary surface and a rigid body where the shape of 

the rigid body is defined geometrically. Possible shapes are flat planes, spheres, cylinders and 

ellipsoids. The main purpose of geometric contacts is to permit LS-DYNA to be coupled with 

other programs that define objects geometrically, (e.g. MADYMO), since it removes the need 

for the analyst to mesh the objects. 

It is recommended that these contact types are not used in normal (uncoupled) analyses as they 

are slow and can produce stability problems where rigid/rigid contact is modelled. 

Page 9.5


INTERIOR CONTACT 

Interior contact is used with meshes of very soft solid elements (eg foams) which are prone to 

invert under severe loading conditions. It is equivalent to a single surface contact in which 

contact segments of a finite thickness are attached to every internal and external solid element 

face. When the elements are severely crushed, these segments contact each other and resist 

further crushing, thus preventing element inversion (negative volumes). 

An alternative method is to coat the outer surfaces with null shell elements, and define contact 

between the null shells. 

OUTPUT 

Two options are available for recovering forces on contact surfaces. 

Time histories of total force against time for surface-to-surface and nodes-to-surface contact 

types can be obtained from the .XTF file via OASYS T/HIS. This output is always generated 

automatically. The forces are time-averaged over the interval between outputs. 

Plots of the contact stress distribution can be obtained by requesting a .CTF file when submitting 

a job. In this case contact stresses are dumped to the .CTF file at the same time as complete state 

data is dumped to the .PTF file. Contact stresses (which are instantaneous values, not timeaveraged) 

can then be plotted by OASYS D3PLOT. 

The total force on a single surface contact is zero by definition, since the action and reaction of 

every penetrating node is included. However, the total force on any subset of a single surface 

contact can be obtained using the *CONTACT_FORCE_TRANSDUCER option. This contact 

type does not generate any force itself: it outputs the total force due to all the contacts on the 

slave set to which it refers. 

CONTACT SEARCH METHODS 

There are two methods used by LS-DYNA for detecting which segment is being contacted by 

each node. Further details are given in the theory manual. In summary, the methods are: 

- Mesh Connectivity Tracking, in which neighbouring segments can be identified because 

they share nodes. When one segment is no longer contacted by a node, the neighbouring 

segments are checked. 

- Bucket sort, in which the 3-D space occupied by the contact surface is divided into cubes 

("buckets"). Nodes can contact any segment in the same bucket or a next-door bucket. 

The Mesh Connectivity method is used by contact types 3, 5, 8, 9 and 10 (unless SHLTHK on 

*CONTROL_CONTACT is non-zero). The main disadvantage is that the mesh must be 

continuous for the contact surface to work correctly. These contacts are rarely used. 

Page 9.6


The Bucket Sort method is applied in all the commonly used contact surfaces. It is much more 

robust but can be slow if the contact surface contains large numbers of segments (or elements). 

The bucket sort is used by types a3, a5, a10, 14, 16 and all single surface types; in addition, types 

3, 5 and 10 use the bucket sort if SHLTHK on *CONTROL_CONTACT is non-zero. 

CONTACT ORIENTATION 

Contact segment orientation defines which side of the surface is "solid" and which is "air". 

Contacting nodes can move freely on the "air" side but penetrations into the "solid" side are 

resisted. If the contact surface is on solid elements, LS-DYNA automatically sets the contact 

orientation correctly whatever the contact type and input method. The rest of this section 

describes what happens with contacts on shell elements. 

All single surface contact types, and types a3, a5, a10, 14 and 16, check for contact on both sides 

of the shell element. This is possible because the contact plane is always offset from the nodal 

plane and the contact depth does not cross the nodal plane. Therefore there is no requirement to 

orient the elements or contact segments in any particular way. 

The orientation of contact types 3, 5 and 10 can be set automatically by LS-DYNA, provided that 

the slave and master surfaces are initially separated by a gap. To do this, either define the contact 

surface by a list of parts and a box, or set ORIEN on *CONTROL_CONTACT to 2. 

Thus, in summary, contact orientation needs to be checked by the user only for contact types 3, 

5 and 10 on shell elements. If defining the surfaces by list of parts, ensure initial gaps are 

present. If defining the surfaces by segments, either create the model with the segments correctly 

oriented or include initial gaps and set ORIEN to 2. 

CONTACT DEPTH 

Contact types 3, 5 and 10 

For contact types 3, 5 and 10, the contact depth is 1 x 10 10 by default (in effect, infinite). 

Therefore any slave node which passes behind a master segment (or vice-versa) will feel a force 

proportional to the distance from the segment. Sometimes this is due to the geometry of the 

situation rather than a genuine case of contact - e.g. Figures 9.2, 9.3. Where the distance is large, 

the force will be large and can cause the model to blow up. To prevent this, it is possible to 

specify a maximum depth, beyond which contact penetrations are to be considered spurious and 

ignored by LS-DYNA. There are two ways to do this: 

either - define the distance as MAXPEN on the *CONTACT cards 

or - set PENCHK (on *CONTACT) to 1. In this case the maximum depth is 

XPENE*thk, where XPENE can be set on *CONTROL_CONTACT (or simply 

left as default = 4.0), and thk is the shell element thickness. For solid elements 

thk is volume/area. XPENE applies to the whole model and cannot be adjusted 

Page 9.7


for individual surfaces. 

Note that SST, MST, SFST, SFST, SFMT (see *CONTACT) do not apply to types 3, 5 and 10. 

If SHLTHK on *CONTROL_CONTACT is non-zero, MAXPEN is ignored and PENCHK is 

always 1. 

Contact types 4, 13, 14, 15, 16, a3, a5, a10 

For these contact types, the contact depth is always limited by element thickness: 

shell elements: 

thk = min [shell thickness, .4 x min side length, .5 x sqrt (area)] 

or thk = user-defined value SST, MST if non-zero. 

solid elements: 

thk = min [volume/area, .5 x sqrt (area)] 

Contact type 26 

This contact type uses a segment thickness of 400 times the shell thickness. Spurious penetrations 

are avoided because the slave node “remembers” from which side it entered the segment. 

CONTACT ON SHELLS: SURFACE OFFSET 

The following applies to all single surface contact types, plus types a3, a5, a10, 14, 16: 

For contacts on shell elements, impacting nodes first feel a resisting force when half a thickness 

from the plane of the shell element. Normally the resisting force is sufficient to maintain the 

node in this position, but if the node were forced to continue its motion, the force would rise as 

the node approached the element, then reverse as the node crossed to the other side of the 

element, reducing to zero as it passed beyond half a thickness from the element. Thus the 

thickness of the shell is accounted for, and contact from both sides of the element is permissible. 

NOTE:Shell elements may not be initially coincident if they are to contact each other. They 

should be offset by the shell thickness. 

For contact types 3, 5, 8, 9 and 10, to which the above does not apply, an impacting node first 

feels a resisting force as it crosses the plane of the element. If the node were forced to continue 

its motion, the resisting force would increase until the maximum penetration depth is reached 

(see CONTACT DEPTH above). Contact can occur from one side only; this is determined by 

segment orientation, if the surface is defined by segments, or by initial gap if either the surface 

is defined by parts or shell elements or ORIEN on *CONTROL_CONTACT is set to 2. Thus 

initial gaps are unnecessary ONLY if the surface is defined by segments and ORIEN is 1 or 0. 

Page 9.8


If SHLTHK on *CONTROL_CONTACT is non-zero, contact types 3, 5 and 10 behave 

differently: the surface is offset from the shell elements by half a thickness (as per the single 

surface types), but contact is from one side only and the contact depth is limited to XPENE x 

thickness (explained under CONTACT DEPTH, above). 

Contact type 26 allows for beam-to-beam contact. Each beam is associated with a contact radius. 

A contact force is generated when the distance between two beams becomes less than the contact 

radius. The contact radius is equal to the square-root of the cross sectional area for Belytschko- 

Schwer (resultant) beams, and the outer diameter or s-direction thickness for Hughes-Liu 

(integrated) beams. 

CONTACT SURFACE STIFFNESS 

Basic Calculation 

The formula for the stiffness of a contact segment is as follows: 

k = fs x Area² x K for segments on 

Volume solid elements 

k = fs x Area x K for segments on 

Minimum Diagonal shell elements 

Area = area of contact segment 

K = bulk modulus of contacted element 

fs = penalty factor (0.1 by default) 

This stiffness calculation is the only reason why material properties have to be defined for rigid 

bodies. 

By default, the lower of the slave and master segment stiffnesses is used both for slave nodes 

penetrating master segments and for master nodes penetrating slave segments. This can be altered 

with the PENOPT flag on the *CONTROL_CONTACT card. 

Choice of Penalty Factor 

The penalty factor (fs) can be changed for all contact surfaces together by entering the new value 

on Control Card 5. Multipliers on this penalty factor can be defined for each of the surfaces 

independently on the contact control cards. It is unwise to raise the factor above 0.1 because 

instability may ensue. See note below on contact timesteps. 

Loadcurve-based Contact Stiffness 

The user can opt to override the automatically calculated stiffness, by using contact types 19, 20 

or 21 and defining a loadcurve which governs the force-penetration behaviour. This allows non- 

Page 9.9


linear and energy-absorbing contact types. Three variants are available. 

1. The loadcurve represents total force on the contact surface vs maximum penetration of any 

node. This is intended for rigid-on-rigid contacts (e.g. occupant on facia) in which the 

complex structural deformation is represented by the contact characteristic - the elements 

themselves do not deform. 

The contact surface must be defined as type 21, with the impacting object (or more finely 

meshed component) being the slave surface and the target (or more coarsely meshed 

component) being the master surface. 

The total force is calculated from the loadcurve, based on the greatest penetration of any slave 

node into the master surface. The force is distributed to all slave nodes currently in contact, 

weighted by the area associated with each node. The areas are calculated on initialisation: 

they are one quarter of the total area of all the contact segments attached to each node. The 

reason for the area-weighting is to make the force distribution less mesh-dependent: if it were 

not done, finely meshed areas would pick up more force because of the greater number of 

slave nodes. Note that the force is not weighted by penetration, so a slave node picks up its 

full share of the force the instant it contacts the master surface. 

2. The loadcurve represents the force on each node vs the penetration of that node. This is the 

most general version of loadcurve-controlled contacts and is available for contact types 19, 

20 and 21. It is intended to allow users to introduce non-linearity into ordinary contact 

surfaces. Examples include: 

- elasto-plastic characteristic to reduce rebound and oscillation. 

- non-linear seatbelt on occupant contact. 

- surface with low stiffness for low forces but high stiffness for high forces; this would 

overcome precision problems in which undetectable penetrations occur in response to 

small loads. 

3. The loadcurve represents the pressure on each node vs the penetration of that node. This is 

similar to variant 2, except that the pressure obtained from the loadcurve is multiplied by the 

surface area associated with the node to obtain the force. The areas are calculated on 

initialisation: they are one quarter of the total area of all the contact segments attached to each 

node. This variant is available for contact types 3 and 10. If type 3 is used both master and 

slave surface will contribute to the total pressure on the surface which may therefore be 

greater than expected. 

Note that the area which multiplies the pressure for each node is the "true-view" area - not the 

area projected onto the target. This leads to an overestimate of force when the impacting 

surface is oblique to the target. 

Page 9.10


Applications include: 

- elasto-plastic characteristic to reduce rebound and oscillation. 

- "soft target" impact calculations in which the deformation of the target is approximated 

by a pressure-vs-depth characteristic; the target itself would then be modelled by a flat 

rigid element. 

Friction and damping can be included as with standard stiffness-based contact surfaces. 

The loadcurve points are (penetration distance, force (or pressure for variant 3)). The optional 

unload stiffness has units force/distance, except for variant 3 which has units pressure/distance. 

The first point on the load curves should be (zero, zero) and all values should be positive. 

PART_CONTACT 

Contact parameters such as stiffness and thickness can be adjusted for individual parts using 

PART_CONTACT. This is useful where soft parts and stiff parts are included in one contact. 

SHELL ELEMENTS OVERLAID ON SOLID ELEMENTS 

If shell elements are overlaid on solid elements, it is the shell elements that count in determining 

contact stiffness and orientation. Note that this is still the case even if the contact is defined by 

a list of parts and the shell part is excluded. 

CONTACT TIMESTEPS 

LS-DYNA computes the timestep at which each contact surface will be stable and prints it to the 

OFT file. However, it does not change the analysis timestep. If the printed contact surface 

timestep is less than the analysis timestep, unstable behaviour may ensue recommend that the 

stiffness of the surface be reduced, either using SFS, SFM on *CONTACT or on 

*PART_CONTACT. 

EFFECT OF SHLTHK 

The flag SHLTHK on *CONTROL_CONTACT (if non-zero) has several important effects on 

contact types 3, 5 and 10: 

- The contact plane is offset from the nodal plane, so initial gaps of at least a material thickness 

must be present. 

- The contact depth is related to element thickness and cannot be controlled directly by the user 

(i.e. MAXPEN, SST, MST, SFST, MFST on *CONTACT have no effect), except by changing 

XPENE on *CONTROL_CONTACT (applies to whole model, not individual surface). 

- The contact search method becomes Bucket Sort, so mesh connectivity is not necessary for 

the contact to work correctly. 

Page 9.11


These effects can cause big differences in model behaviour, so it is strongly recommended that 

for general use SHLTHK is set to zero. 

NULL SHELLS 

Shell elements made of *MAT_NULL can be used to coat solid element meshes to help stabilise 

the contacts. These are often recommended if the solids are soft e.g. foams. 

RECOMMENDED INPUT PARAMETERS 

There are many input parameters for contact surfaces in LS-DYNA. OASYS recommend the 

following: 


Leave all parameters to take the default settings, except: 

- If compatibility with OASYS DYNA3D 5.1 is required, set PENOPT = 2 

- ORIEN can be set to 2 if all surface-to-surface contacts have initial gaps. 

*CONTACT 

Leave all parameters to take the default settings, except: 

- SPR, MPR should both be set to 1 to allow viewing of contact surfaces in OASYS D3PLOT 

(also requires user to request a Contact Force file when submitting the job). 

- FS, FD: generally set both of these to the same value (OASYS suggest 0.2 if no other 

information is available). 

- SST, MST (applies only to contact types 4, 13-16, a3, a5, a10 on shell elements). Can be 

adjusted if required but generally leave as default. 

- NFLF, SFLF, NFLS, SFLS (contact types 8 & 9 only). Must be non-zero or the contact will 

break apart immediately. If the contact is required not to break apart, input high values (e.g. 

1E8). 

- NEN, NES (contact type 8 only). Suggested value 2.0. 

- MAXPEN (contact types 3, 5, 10). OASYS recommend that a non-zero value be set for all 

type 3, 5 and 10 contact surfaces. Typical values would be 1 to 2mm for metal-on-metal 

contact; 5 to 10mm for contacts involving foams or other soft materials. 

Page 9.12


SUMMARY TABLE 

The contact types can be grouped as follows: 

Group 

A B C D 

Can be defined by list of parts yes yes yes yes 

Search method Mesh 

Connectivity 

Bucket Sort Bucket Sort Mesh Connectivity 

Contact from both sides no no yes no 

Orientation of segments 

important 

yes yes no yes 

Default contact depth 10000000000 4 x thickness 0.4 x thickness 

Type 26: 400 x 

thickness 

Variable which limits contact 

depth 

infinite 

MAXPEN XPENE SST, MST (ON 

LOADCURVE) 

Contact plane offset from nodes no yes yes no 

Initial gaps essential no yes yes no 

A: Types 3, 5, 10 (SHLTHK = 0) B: Types 3, 5, 10 (SHLTHK = 1) 

C: Types 4, 13, 14, 15, 16, a3, a5, a10, 26 D: Types 19, 20, 21 

ERRORS AND WARNINGS 

Kinematic Constraint Surfaces 

Surface types 1, 2, 6, 7, 17 and 18 work by imposing motion on nodes to maintain contact 

between the surfaces. This will clash with any other motion imposed by features such as rigid 

bodies, restraints, constraints, stonewalls, other tied surfaces, etc. No more than one such feature 

should be present at any given node. 

Escape from Concave Surfaces 

Where neighbouring contact segments form a concave surface, there would appear to be a wedgeshaped 

region of no-man's land behind the edge which belongs to neither one segment nor the 

other, and in which nodes may therefore lose contact with the surface. LS-DYNA prevents this 

by adding a 2.5% margin to the width of each segment (shown shaded in Figure 9.4). Thus node 

A can pass from one segment to the other without losing contact. 

If the penetration is very great (node B in Figure 9.4) the 2.5% margin may be insufficient - there 

Page 9.13


is still a wedge of no-man's land through which node B can lose contact with the surface and 

escape. 

This error occurs only where contact forces are very large or the stiffness of the contact surfaces 

is very low. 

The symptom is that nodes appear to escape through the contact surface after crossing from one 

segment to another. 

Escape can also occur during contact with very soft or very thin shell elements, or with very fast 

impact speeds, even if the surfaces are not concave. In this case, the node simply penetrates too 

far and is set free. 

The cure is to increase the stiffness of the contact surface. One easy way to achieve this with 

group C surface types is to set the SOFT flag to 1 in the *CONTACT cards. This flag causes the 

“soft constraint” contact formulation to be used, which is a penalty method where the maximum 

stable contact stiffness is chosen for each penetrating node. 

For type 13 contacts the 2.5% margin can be increased (MAXPAR on *CONTACT). 

Precision 

Figure 9.4 Escaped Node 

If the equilibrium penetration of one surface into another (i.e. the force divided by the stiffness) 

is too small to be detected, difficulties can arise. A typical symptoms is very noisy contact force. 

In this case the stiffness of the contact surface should be reduced. 

Over-Fast Impact 

In one timestep a node penetrates so far into the surface that the contact force is very large and 

shoots the node out again. If this occurs, the stiffness of the contact surface should be reduced. 

Page 9.14


It can be difficult to detect very rapid penetrations of this type since they may only occur over a 

few time-steps. It is for this reason that the summary contact forces reported to .XTF file are 

averaged over the time between data points: spikes at inter-data points are detected, albeit with 

attenuated force. Contact forces reported to the .CTF file are instantaneous and will almost 

always miss rapid spikes of force. 

Shell Edge Contacts 

In complex contact situations (e.g. crash analysis) it is possible for the edges of shell elements 

to come into contact with other Shell elements. This often leads to energy jumps and unrealistic 

local deformation. Where the likelihood of edge-on contact is great, it is better to use a nodeson-surface 

contact type. *CONTACT AUTOMATIC-GENERAL is better able to deal with these 

situations. 

Page 9.15


Page 9.16


10.0 RESTRAINTS & CONSTRAINTS 

This section describes the options for restraining nodes (clamping) or constraining them (tying 

them to other nodes). Similar options are available for rigid bodies, but these are entered in a 

different way and are described in Section 8. 

RESTRAINTS 

Restraints work by setting the accelerations of nodes to zero in the restrained directions. 

The usual method is to use SPC Restraints (*BOUNDARY_SPC) with defined coordinate 

systems (*DEFINE_COORDINATE_SYSTEM). The coordinate system can be aligned with the 

global x,y and z axes, or not, as required. 

Restraints in global x, y and z directions can also be entered on the node cards. 

CONSTRAINTS 

Any number of nodes can be tied together in any of the global x, y and z directions - see Section 

3.31 of this manual. Constraints work by summing the forces on the constrained nodes, summing 

their masses, and hence calculating the motion of the constrained set. This motion is then 

imposed on all of the constrained nodes. There is no "master" node which the other nodes have 

to follow - all the nodes in the set are treated equally and overall equilibrium of the constraint set 

is preserved. 

Another type of constraint is *CONSTRAINED_SPOTWELD. Two nodes (which must not be 

coincident) are linked by a massless rigid bar. Failure forces can then be defined at which the 

spotweld breaks and the nodes become free. If more than two sheets are connected, use 

*CONTRAINED_GENERALISED_WELD_SPOT. 

Other features which work by imposing motion on the nodes (such as rigid bodies, restraints, etc) 

should not be applied to constrained nodes. In particular, it is wrong to define the same nodal 

degree of freedom in more than one constraint set; both sets attempt to impose a different motion 

on the same node. This does not cause the program to crash, but the supposedly constrained 

nodes drift apart. Instead, all the nodes which are required to move together should be defined 

in a single constraint set. The global x, y and z degrees of freedom are treated independently, so 

it is possible to restrain a node in x and constrain the same node in y, etc. 

It is not possible to constrain nodes in directions other than global x, y or z, nor to constrain 

rotational degrees of freedom. 

Page 10.1


Page 10.2


11.0 ENERGY DATA 

The energy data which is printed in the .LOG and .OTF files forms a useful check on an analysis. 

The following equation should hold at all times during an analysis. 

KE + IE = KE o + EW 

Where KE = current kinetic energy 

IE = current internal energy 

KE o = initial kinetic energy 

EW = external work 

Internal energy includes elastic strain energy and work done in permanent deformation. External 

work includes work done by applied forces and pressures but currently excludes work done by 

velocity, displacement or acceleration boundary conditions - so the equation above will appear 

not to hold if these features are used. By default energy absorbed by contact surfaces is excluded. 

In particular, work done against friction can be significant and energy being dissipated in this 

way will appear to be lost. However, this energy can be included by setting SLTEN to 2 on 

*CONTROL_ENERGY. Energy associated with hourglassing is also excluded by default, but 

can be included (HGEN on *CONTROL_ENERGY). 

The terms in the equation can all be plotted using OASYS T/HIS. If the equation does not hold 

the user should suspect an error. If the left hand side of the equation rises above the right hand 

side, energy is being introduced artificially - for example, by numerical instability, or the sudden 

detection of artificial penetration through a contact surface. The latter condition is often shown 

by sudden jumps in the total energy. If the left hand side falls below the right hand side, energy 

is being absorbed artificially, perhaps by excessive hourglassing or by stonewalls or overcompliant 

contact surfaces. Sometimes this can be due to a genuine physical effect whose energy 

is not countedin the balance. A typical example is friction on contact surfaces. This can be 

remedied using *CONTROL_ENERGY as described above. 

The energy in each material can also be plotted using OASYS T/HIS. If the total energy 

indicates an error, plotting by material can sometimes indicate where the problem is occurring. 

Page 11.1


Page 11.2


12.0 TIMESTEP CONTROL 

The timestep in LS-DYNA is generally limited by stability. Usually, the timestep falls during 

an analysis as elements become deformed. It is also possible for the timestep to rise. LS-DYNA 

automatically calculates the largest timestep which can be used without triggering numerical 

instability; it is not possible to force the code to use a timestep larger than this. It is, however, 

possible to force the code to use a timestep smaller than the calculated value, either by defining 

a multiplying factor less than the default value of 0.9 (SCFT on *CONTROL_TIMESTEP), or 

by specifying a timestep-vs-time loadcurve (LCTM on *CONTROL_TIMESTEP). 

Instability (shown by rapidly rising energy and a "floating overflow" error) will occur if the 

period of any mode of deformation in the model is less than π times the timestep. Thus the 

timestep must divide the period of the highest mode by at least π. Generally the highest mode 

is a single element mode, i.e. oscillation of a single brick, shell, beam or spring element. 

LS-DYNA checks all elements when calculating the required timestep. The timestep can be 

estimated roughly using the formula 

ìt = 0.9 L/c (solid, shell, beam) 

where l is the smallest element dimension and c the speed of sound in the material. Shell 

thickness and beam section dimensions are ignored when finding l. Rigid elements are not 

included. 

More accurate estimates can be obtained using l and c instead of l and c as follows: 

L = Volume/Area of largest surface (solid elements) 

L = as per ISDO on *CONTROL_TIMESTEP. 

c = (E/ρ) 

E = K + 4G/3 = E(1-ν)/[(1+ν)(1-2ν)] 

It is possible for flexure modes of Belytschko-Schwer beams to control the timestep especially 

if they are short in comparison to their section dimensions. In this case, 

t =014l 2 (A(12r + 1)/I(3r + 1)) 

c' 

Where A = cross-sectional area 

I = maximum of I ss, I tt, J 

r = I/(Al 2 ) 

Page 12.1


For spring elements the calculation is: 

t = 2(mk) 

Where m = m 1m 2/(m 1 + m 2) 

m 1,m 2 = mass of nodes 

k = current spring stiffness 

For dampers it is 

ìt = 0.1m/λ 

Where λ = damping constant 

m = as above 

For more details see Section 19 of the Theory Manual. 

On commencing the solution phase and also on restart LS-DYNA reports the 100 elements with 

the smallest timesteps to the .OTF file. There is also an option (IPNINT on 

*CONTROL_OUTPUT) to output the initial timestep of all the elements in the model. 

In most problems the stable timestep selected by LS-DYNA is small enough not to affect 

accuracy (i.e. use of a smaller timestep would produce the same answers). 

Exceptions occur when the highest modes in the model (i.e. single element modes) have a 

significant effect on the results, e.g. mass-spring models and shock wave problems. In these 

cases it is usually beneficial to reduce the timestep. 

Three options are available for preventing the timestep falling below a given value (all of these 

are on *CONTROL_TIMESTEP): 

TSLIMT (applies only to shell elements of material types 3, 18, 19 and 24). This reduces 

the Young's Modulus of elements which would otherwise demand a timestep less 

than TSLIMT. The timestep for the whole model is then prevented from falling 

below TSLIMT. This can be dangerous: if the critical element is not a shell 

element of the material types given above, the model may go unstable and the run 

may then crash. 

DT2MS When set to a negative value, this tells LS-DYNA to add mass to any element 

which would otherwise demand a timestep less than SCFT*DT2MS. Because 

this option applies to all element classes (except spring elements) and material 

types, it should be used in preference to TSLIMT. Use with ENDMAS on 

*CONTROL_TERMINATION. 

Page 12.2


ERODE (with DTMIN on *CONTROL_TERMINATION) Elements whose timesteps fall 

below SCFT*DTMIN*DTSTART (where DTSTART is the initial timestep) will 

be deleted provided that ERODE is set to 1. The disadvantage of this is that the 

eroding contact types must be used if solid elements are present, with consequent 

increase in memory and CPU requirements. Also the holes left by the deleted 

elements can cause contact problems. If DTMIN is non-zero but ERODE is 

zero, the run will simply terminate if the timestep falls below 

DTMIN*DTSTART. 

Note that none of the above options apply to Spring elements. For any Spring elements which 

may control the timestep, it is recommended that lumped masses be added to their nodes. In 

previous versions of LS-DYNA it was possible to force LS-DYNA to ignore spring elements 

when calculating the timestep. This option was considered dangerous and has been discontinued. 

Optimising the Timestep for Impact Models 

Simply enter the required timestep (with a negative sign) as DT2MS on 

*CONTROL_TERMINATION. LS-DYNA will add mass as required to bring the timestep up 

to SCFT*DT2MS (N.B. SCFT is usually 0.9; it is advisable to allow for this when selecting a 

value of DT2MS). Mass is added only to those elements whose timestep would otherwise have 

been less than the specified value. The amount of mass added can be checked in the LOG and 

OTF files. Clearly the more mass added, the less accurate the calculation; it is up to the analyst 

to decide how much added mass is allowable. To reduce the added mass, reduce the specified 

timestep. 

Subcycling 

Most models contain elements of a range of sizes, and generally the timestep for the whole model 

is controlled by the smallest element. Thus CPU time is wasted in recalculating strains and 

stresses in the larger elements more often than is required for stability. Subcycling overcomes 

this by dividing the elements into groups by timestep, and by using a different timestep for each 

group. If the smallest timestep in the model is DT, the timesteps for the groups are DT, 2DT, 

4DT, 8DT, 16DT and 32DT. (Further explanation is given in the Theory Manual, Section 21.2). 

Subcycling offers a most significant reduction in CPU requirement when there are relatively few 

small elements, and the bulk of the elements have a stable timestep at least twice that of the 

smallest element: for example, if one small region of a model is meshed much more finely than 

the remainder. In a typical crash model, the mesh size is well planned and a large proportion of 

the elements have a timestep within a factor of two of the minimum timestep. In these cases, 

subcycling is unlikely to reduce CPU cost significantly and may even increase it, especially on 

vector machines. To activate subcycling in a model, include *CONTROL_SUBCYCLE in the 

input file. No further input is required. 

Page 12.3


Mass Scaling 

For quasi-static solutions, optimum efficiency is obtained by arranging for all elements in the 

model to require the same timestep. This can be achieved by adding or subtracting mass from 

each element. To perform an analysis of this type, enter a positive value of DT2MS on 

*CONTROL_TIMESTEP. The mass of every element in the model will then be adjusted such 

that the timestep is SCFT*DT2MS (SCFT is normally 0.9). Note that the analyst must still select 

a suitably long event time for the simulation to ensure that the behaviour is sufficiently quasistatic. 

Note also that if DT2MS is set to a negative value, masses are changed only for those elements 

whose timestep would otherwise be less than the desired timestep. With DT2MS positive, the 

masses of all elements are changed. 

Page 12.4


13.0 DYNAMIC RELAXATION 

DESCRIPTION 

Dynamic relaxation is a method of obtaining static solutions in LS-DYNA. The method differs 

from the standard transient solution only in that damping is applied to all the nodes in the model 

and the analysis terminates when convergence is reached. Thus, if the loading is constant, 

oscillations will be damped out and a static solution obtained. Dynamic relaxation can be 

performed before a transient analysis in order to include preload, or after a transient analysis to 

represent spring-back and find residual stresses. It is not generally appropriate for quasi-static 

problems, in which solutions over a continuous range of displacements are required. 

HOW TO SPECIFY DYNAMIC RELAXATION 

On *CONTROL_DYNAMIC_RELAXATION, input a checking interval (NRCYCK), a 

convergence tolerance (DRTOL) and a damping constant (DRFCTR). It is also necessary to 

specify dynamic relaxation either using IDRFLG or by stating that at least one of the load curves 

should act during dynamic relaxation (SIDR on *DEFINE_CURVE) 

CHOICE OF CONSTANTS 

The checking interval is the number of cycles (timesteps) between checks for convergence. The 

checking process is cheap so there is very little cost penalty in specifying frequent checks. 

However, information (including convergence progress) is written to the .LOG file at every 

check; very frequent checks will result in .LOG files which are inconveniently large, while 

infrequent checks result in a lack of information for diagnostic purposes and wasteful overrun 

past the convergence point. The default interval of 250 cycles is generally adequate. 

The convergence tolerance is the convergence parameter at which the solution is deemed to be 

complete. In previous versions of LS-DYNA the convergence parameter was defined as: 

C 

C 

Current distortional k.e 

Maximum distortional k.e 

from version 6.1 onwards this definition has been modified to take into account the internal 

energy. 

Current distortional k.e Current i.e 

Maximum (distortional k.e i.e) 

This parameter is written to the OTF file at each check. 

Page 13.1


The distortional kinetic energy is defined as: 

Distorsional 

k.e 

Total 

k.e 

Total mass (mass averaged velocity) 2 

Typical values are 1E-3 (loose) - 1E-6 (tight) convergence. The degree of error associated with 

a given convergence tolerance depends on the structure and the loading history. If only 

displacement results are required, a looser tolerance may be used than if stresses are wanted. For 

preload applications a loose tolerance is generally sufficient. 

The damping constant is a number which multiplies all nodal velocities at each timestep. Its 

value must lie between 0 and 1 (the closer to 1, the less the damping). It is important to choose 

the damping constant carefully; ideally the solution should be critically damped. Over damping 

will result in the calculation taking too long to converge, sometimes by several orders of 

magnitude. Under damping will result in overshoot, sometimes resulting in large errors. 

Overshoot can also cause errors with path-sensitive systems, e.g. models involving friction. 

To calculate the correct damping constant, it is necessary to estimate the lowest natural frequency 

of the structure, and the solution time step. The damping constant (k) is given by: 

k = 1 - 2cω n dt 

where c = desired fraction of critical damping (normally 1.0) 

ω n = lowest natural frequency of oscillation (rad/s) 

dt = timestep 

LOADING 

Any of the LS-DYNA loading methods involving load vs time functions can be used (e.g. point 

or pressure loads, prescribed velocities, etc). Initial velocity conditions cannot be used to load 

the dynamic relaxation phase; the velocities are initialised to zero, and user-specified initial 

velocities are stored for use in any transient analysis which follows the dynamic relaxation. 

Load curves may be set to act during dynamic relaxation only, during normal transient analysis 

only, or during both phases (SIDR on *DEFINE_CURVE). Thus it is possible to use different 

methods for each phase. Load curves for dynamic relaxation should contain a constant load to 

allow a converged solution to be reached. It is good practice to ramp the load initially to avoid 

sudden loading and over-excitation of higher modes. 

2 

Page 13.2


Figure 13.1 Typical Load vs Time Curve for Dynamic Relaxation 

TERMINAL VELOCITY 

If a constant load is applied to an unrestrained dynamic relaxation then the body will reach a 

“rigid body” terminal velocity that is given by the following equation. 

V term 

F dt k 

m (1 k) 

where F = desired fraction of critical damping (normally 1.0) 

dt = timestep 

k = damping constant 

m = mass of body 

Although this calculation may not appear to be of much use in itself it can be used as a guide to 

the velocity that will be obtained in the analysis if parts have to move together. 

OUTPUT 

By default no output (except convergence data in the .LOG and .OTF files) is produced during 

dynamic relaxation, and the time is reset to zero when convergence is reached. Complete State 

and Time History data are always output on convergence. The subsequent transient analysis will 

then show non-zero displacements and stresses (the static solution) at time zero. The finish time 

specified on *CONTROL_TERMINATION does not apply to the dynamic relaxation phase. 

The finish time will determine how long the subsequent transient phase lasts. A finish time of 

zero will give a static solution only. 

To obtain plot file information during dynamic relaxation, include a 

*DATABASE_BINARY_D3DRFL card. A binary file (jobname.rtf) will then be written, 

containing plot states at each convergence check. This file can be read into OASYS D3PLOT 

7.0 for viewing, and in structure is identical to the PTF file. 

Page 13.3


To obtain time-history information, set IDRFLG to -1. Time history results will then be written 

to the THF and XTF files. See note in Keyword manual under 

*CONTROL_DYNAMIC_RELAXATION. 

CONVERGENCE BEHAVIOUR 

Typical convergence behaviour for a successful dynamic relaxation run is shown below. Under 

damped and over damped responses are shown for comparison 

Figure 13.2 Convergence Behaviour 

The most common problem with dynamic relaxation is that the solution fails to converge. Such 

cases can be divided into two types: 

a) the solution never starts to converge 

b) the solution partly converges but never reaches the convergence tolerance. 

Figure 13.3 Convergence 

Page 13.4


Type (a) is most often caused by an unresisted (but loaded) mode of deformation; it can also be 

caused by severe over-damping (this can sometimes occur if the lowest mode has not been 

identified). 

Type (b) is most usually caused by hourglassing. It is often beneficial to select stiffness 

hourglass control (enter 4 in column 30 of material card 1). Type (b) can also be caused by very 

high modes of oscillation such as single element modes. These are immune to dynamic 

relaxation unless the timestep is reduced (a factor of 5 below the default timestep is generally 

sufficient). 

When solutions fail to converge, it may be useful to plot time history and/or complete state 

results to determine the cause of the problem. 

AUTOMATIC CONTROL OF DYNAMIC RELAXATION 

This option (IRELAL and EDTTL on *CONTROL_DYNAMIC_RELAXATION ) attempts to 

adjust the damping value continuously, according to the current rate of convergence. See Theory 

Manual, section 28 for more details. 

Page 13.5


Page 13.6


14.0 HOURGLASSING 

Certain modes of deformation of LS-DYNA solid and shell elements are zero energy modes and 

have no stiffness. They typically give a zig-zag appearance to a mesh (see Figures 14.1 and 

14.2); this is known as hourglass deformation. It can swamp the results of an analysis. 

Hourglassing can affect brick and quadrilateral shell elements, but not triangular shells or beams. 

Hourglass-mode deformation is resisted by a viscosity; this is calculated automatically by the 

code. Although it is possible to change the default values (card 1 of each material) it is very 

rarely necessary or desirable to do so. 

Good modelling practice normally prevents hourglassing becoming significant. The general 

principle is to avoid concentrating load on a single node - spread the load over several 

neighbouring nodes. 

Hourglassing can be a problem with small displacement situations, particularly when dynamic 

relaxation is used. In these cases it is often beneficial to opt for the stiffness method of hourglass 

control instead of the viscous method - include an *HOURGLASS card with IHQ set to 4. 

However, this may over-stiffen results in large deformation problems. 

Figure 14.1 Normal Mesh Figure 14.2 Hourglassing 

A more generally applicable solution to hourglassing problems is to opt for fully integrated 

elements (specified on *SECTION_SOLID or *SECTION_SHELL). These are, however, much 

more costly than the default elements. 

Page 14.1


Page 14.2


15.0 IMPOSED MOTION 

Certain features in LS-DYNA work by imposing motion on nodes. If two different features 

attempt to impose motions on the same node, problems will arise. Not all such clashes give rise 

to error messages. The problem rarely causes the analysis to crash but almost always gives 

wrong results. Examples of "imposed motion" features are: 

*BOUNDARY all types, including all restraints and displacement, velocity and 

acceleration boundary conditions 

*CONSTRAINED all types including SPOTWELD but not JOINT 

*CONTACT types 1, 2, 6, 7, 17 and 18 but not other types 

Rigid bodies (i.e. elements made of parts which reference a *MAT_RIGID) 

*INTERFACE 

*RIGIDWALL 

No node should have more than one of the above attached to it. For example, it is an error to 

include the same node on two rigid bodies, or to attempt to impact a rigid body against a 

stonewall (but note possibility of using RWPNAL on *CONTROL_CONTACT), or to include 

a restrained node in a set of constrained nodes, or to spotweld onto a rigid body. However, the 

x, y and z degrees of freedom are treated independently, and it is possible, for example, to 

restrain a node in x and constrain the same node in y. 

Some error checking is done for clashes between "imposed motion" features, but the checking 

is not comprehensive. A typical symptom of the problem is that supposedly constrained nodes 

drift apart. 

Options are available for rigid bodies which overcome certain of these problems - see Section 

7. 

The most commonly used contact surface types (3, 13 and 5) do not impose motion and hence 

do not suffer from the problems described above. They can be used with rigid bodies and can 

be overlapped such that nodes are on more than one contact surface. 

Page 15.1


Page 15.2


16.0 AIRBAGS 

INTRODUCTION 

Airbags can be simulated in LS-DYNA by defining an enclosed mesh of membrane elements as 

a “control volume”. A mass flow rate of inflator gas, and parameters to control the venting, are 

also defined. LS-DYNA uses thermodynamic relationships to determine the internal pressure in 

the control volume based on the mass and temperature of inflator gas present and the volume 

enclosed. It then applies that pressure to the membrane elements, causing the airbag to inflate. 

Airbags are not the only application of control volumes. Another common application is the 

modelling of inflated tyres. In this case, a toroidal control volume is defined to represent the tyre 

and the venting is set to zero. 

INPUT DATA 

The material model most often used to represent airbag material is type 34 (*MAT_FABRIC). 

An example of typical input data for this material is given below. The units for all examples 

given in this chapter are millimetres, seconds, Newtons and Tonnes. 

*MAT_FABRIC 

$ fabric 

1 8.000E-10 300.00000 300.00000 300.00000 0.1000000 0.1000000 0.1000000 

136.000000 136.00000 136.00000 1.0000000 0.0000000 0.0000000 0.0000000 0.0500000 

0.00000000 0.0000000 0.0000000 0.0000000 0.0000000 0.0000000 0.0000000 0.0000000 

0.00000000 0.0000000 0.0000000 0.0000000 0.0000000 0.0000000 0.0000000 0.0000000 

0.00000000 0.0000000 0.0000000 0.0000000 0.0000000 0.0000000 0.0000000 0.0000000 

Note: 

! The flag to eliminate compressive stresses (card 2, 4th entry) should be set to 1. This ensures 

that the elements have no resistance in compression. 

! Some damping (card 2, last entry) is recommended. A typical value is 0.05. 

! Typical fabrics would have stiff properties in the fibre directions at 0 and 90 degrees, but 

would be much less stiff at 45 degrees. This can be modelled to some extent by setting the 

Poisson’s ratio high, so that the shear modulus is low. 

The control volume itself is defined using the *AIRBAG keyword. For most applications, the 

*AIRBAG_SIMPLE_AIRBAG_MODEL or the *AIRBAG_WANG_NEFSKE types should be 

used. An example of typical input data for the Wang-Nefske airbag is given below. 

Page 16.1


*AIRBAG_WANG_NEFSKE 

$ SID ][ SIDTYP ][Rbody ID][ V scale][ P scale][ V init ][mass dmp][ SPSF ] 

1 1 0 1.0 1.0 0.000E+00 5.000E+01 0.7 

$ Cv ][ Cp ][ Temp ][LC temp ][LC mflow][tank vol] 

8.5e8 1.1e9 800 1 

$ C23 ][ LCC23 ][ A23 ][ LCA23 ][ CP23 ][ LCCP23 ][ AP3 ][ LCAP23 ] 

1.0 1500. 

$P ambint][rho amb ][ G conv ] 

1.009E-01 1.200E-12 1.000E+00 

$ IOC ][ IOA ][ IVOL ][ IRO ][ IT ][ LCBF ] 

*SET_PART_LIST 

1 

1 5 

$ 

$ ====================== LOAD CURVES ====================== 

$ 

*DEFINE_CURVE 

1 

$ massflow into airbag 

$ Time (s) mass flow rate (kg/s) 

0.00000E+00 0.00000E+00 

0.010000 1.8e-3 

0.040000 0.0 

0.10000 0.0 

Note: 

! The easiest way to specify the elements that make up the airbag is with a part list, referred to 

on card 1, first entry. 

! Some damping is recommended (card 1, last two entries). 

! Always define GC as 1.0 (card 3, 3rd entry) 

! Cp, Cv, T and the mass flow rate normally come from a tank test analysis programme which 

back-calculates these parameters from the pressure time-history in the tank. 

! The mass flow rate is defined as a function of time using a curve as in the example. The units 

are Tonne/sec in this example. It typically peaks at about 2E-3 Tonne/sec. 

FOLDING AIRBAGS 

Although real airbags are initially folded, it is not always necessary to use a folded mesh when 

simulating them. With in-position occupant studies, the airbag is usually fully inflated by the time 

the occupant contacts it, so that the unfolding process has little effect on occupant interaction. 

Unfolded or partially folded meshes are easier to create and use than fully folded meshes. Apart 

from the extra time required to fold an airbag mesh, additional CPU time is needed to analyse 

them due to the finer mesh and internal contact. 

Initially unfolded airbags are typically flat discs, with a spacing of around 1.0mm between the 

front and back layers. In such cases the occupant’s arms may be initially penetrating the outer 

regions of the airbag. One way of avoiding initial contact is by introducing a small number of 

initial folds so that the arms are outside the airbag. For example, there might be a 90 degree 

Page 16.2


vertical fold on either side of the module, with the outer portions of the bag initially pointing 

towards the occupant. Another way is to use an initially shrunken airbag and the “reference 

geometry” facility (see later). 

However, in many cases the interactions of interest occur as the airbag is unfolding, for example 

where the occupant is out of position or when the behaviour of the airbag module is being 

studied. Such simulations must use a fully folded airbag mesh. 

OASYS PRIMER contains special features to create a folded airbag mesh from an unfolded one. 

The PRIMER manual contains a tutorial. Here are some tips: 

! As well as straight mesh lines along the fold positions, also make the next-door mesh lines 

straight and parallel to the folds 

! When creating the unfolded mesh in the normal pre-processor, space the two layers slightly 

more than one fabric thickness apart. 

! The fold thickness should typically by slightly more than one fabric thickness 

! Adjust the fold “scale factor” to achieve parallel lines at the folds 

! Use thorough visual checking of the folded mesh in PRIMER to check that there are no initial 

penetrations. 

RUNNING FOLDED MODELS 

Folded airbags must have a single-surface contact defined to prevent one part of the airbag 

penetrating another. The recommended contact type to use is 

*CONTACT_AIRBAG_SINGLE_SURFACE, which has been specially formulated for airbag 

unfolding. 

Even when an airbag has been folded and checked carefully in PRIMER, a number of initial 

penetrations are often detected: check for warnings in the otf file. There should be no initial 

penetrations if the airbag contact is to work correctly. Initial penetrations can be avoided by 

controlling the contact segment thickness as a function of time via a load curve. The load curve 

is defined using the LCIDAB in the *CONTACT cards. Typically the curve will begin at 0.3 to 

1.0 times the real fabric thickness, rising to 1 to 2 times the fabric thickness at 1-2 millisec, and 

remain constant thereafter. 

Use trial and error to find the maximum value of the initial thickness that prevents warnings. If 

the value is less than about 0.1mm the folded mesh is probably not good enough. 

Usually, the timestep has to be reduced to prevent contact problems as the bag unfolds. This is 

most important in the first millisecond; there is less need for a small timestep as the unfolding 

process continues. The timestep can be controlled by a load curve on *CONTROL_TIMESTEP. 

The ideal curve is problem-dependent and must be found by trial and error. With very tightly 

Page 16.3


folded bags, an initial timestep as low as 0.1 microsec may be necessary, rising to the LS-DYNA 

default by 5 millisec. 

REFERENCE GEOMETRY 

By default, the undeformed state of the fabric elements is defined by the initial geometry. 

However, this is not always wanted. 

By using the airbag reference geometry feature, it is possible to define the flat, unfolded mesh 

geometry separatety from the initial geometry. LS-DYNA then compares the current geometry 

of an element with the reference geometry, instead of the undeformed geometry, to calculate the 

strains and stresses in an element. Stresses are zero until an element size reaches that of its 

equivalent in the reference geometry. 

There are two main reasons for using this feature: 

! Folding the mesh distorts the elements around the fold lines so that the initial geometry is 

inaccurate. This can lead to an incorrect shape when the bag is inflated unless the reference 

geometry is used. 

! A “shrunken” unfolded bag may be used to avoid initial contact with the occupant or to 

achieve a reasonable initial volume. The airbag will inflate to the correct size if it is defined 

using the reference geometry. 

The coordinates of the airbag nodes in the folded or reduced state is included under *NODES as 

usual. The coordinates of the same nodes in the flat, full-size state are given under 

*AIRBAG_REFERENCE_GEOMETRY. For reduced size airbags, use 

*AIRBAG_REFERENCE_GEOMETRY_RDT. This sets the timestep based on the reference, 

not the reduced state. 

If the fabric is defined as orthotropic, the angles are relative to the reference geometry: this 

simplifies the definition for folded airbags. 

JETTING 

In a real airbag, the pressure on the portions of fabric directly in front of the inflator will be 

higher than the pressure on other parts of the bag, because the fabric in front of the inflator feels 

momentum forces from the gas entering the bag. However, the internal pressure in an LS-DYNA 

control volume is constant throughout the volume at any given time. 

LS-DYNA can simulate the effect of the momentum forces from the gas that rushes out of the 

inflator. It does this by applying extra forces to nodes that are in the inflator’s line-of-sight. The 

user defines the inflator position and direction, and a “cone angle” over which the forces are to 

be applied. The jetting forces are calculated automatically from the mass inflow and gas 

Page 16.4


parameters and applied over the cone angle using a Gaussian distribution, with the highest forces 

applied to nodes along the centreline of the cone. 

Virtual origin 

(Focus) 

Hole diameter 

Pressure is applied to surfaces that are 

in the line of sight to the virtual origin 

Airbag 

Gaussian profile 

Cone center line 

Note that the jetting forces are only an approximation and do not address most of the gas 

dynamics issues. 

The airbag types to use with the jetting model are *AIRBAG_WANG_NEFSKE_JETTING and 

*AIRBAG_WANG_NEFSKE_MULTIPLE_JETTING. The only difference between them is that 

the pressure distribution over the cone angle is user-defined by a load curve in the 

MULTIPLE_JETTING type, instead of being automatically defined as a Gaussian curve. 

*AIRBAG_WANG_NEFSKE_JETTING 

$ SID 1[ SIDTYP ][Rbody ID][ V scale][ P scale][ V init ][mass dmp][ SPSF ] 

1 1 0 1.0 1.0 0.000E+00 5.000E+01 0.7 

$ Cv ][ Cp ][ Temp ][LC temp ][LC mflow][tank vol] 

8.5e8 1.1e9 800 1 

$ C23 ][ LCC23 ][ A23 ][ LCA23 ][ CP23 ][ LCCP23 ][ AP3 ][ LCAP23 ] 

1.0 1500. 

$P ambint][rho amb ][ G conv ] 

1.009E-01 1.200E-12 1.000E+00 

$ IOC ][ IOA ][ IVOL ][ IRO ][ IT ][ LCBF ] 

$ jet focal point x, y and z ][ jet vector head x, y and z ][cone ang][ beta ] 

0.000E+00 0.000E+00-7.000E+00 0.000E+00-0.300E+00 0.300E+00 1.000E+00 

$ secondary jet focal x y z ][part set][cutoff a] 

2 3.000E+01 


1 

1 


2 

1 

$ ====================== LOAD CURVES ====================== 

*DEFINE_CURVE 

1 

$ massflow into airbag 

$ Time (s) mass flow rate (kg/s) 

0.00000E+00 0.00000E+00 

0.010000 1.8e-3 

0.040000 0.0 

0.10000 0.0 

Page 16.5


Note: 

! The parts affected by jetting are listed in a part set. Only the include the front face of the 

airbag—otherwise the rear face will be pushed out instead. 

! The jet focal point needs to be some distance away from the airbag, to avoid high forces being 

concentrated on a single element. 

! The direction from the focal point to the jet head defines the direction of the jetting forces. 

! The angle is the cone semi-angle in radians. 

CALIBRATION OF JETTING AIRBAGS 

The jetting force is calculated automatically from thermodynamic equations. These do not take 

account of the form of the orifice and many other factors. The total force applied by the model 

jet must be calibrated to allow for this. Typical drivers-side airbag inflators have peak reactions 

around 0.5 to 2kN. 

The jetting force is not output directly by LS-DYNA it must be found using a separate model. 

Use the same mass flow curve and thermodynamic data but double the size of the bag to avoid 

developing significant overpressure. Apply the jet to a rigid back face, supported on stiff springs. 

Sum the forces in the springs using T/HIS. This is the jetting force. The “efficiency factor” in the 

model should then be scaled so that the peak force is correct. 

Jetting can alter the way in which an airbag deploys, especially during the initial stages of 

inflation However, it has a minimal effect on the airbag pressure time-history. 

Spring 1E4 N/mm 

F 

B 

A 

2 x actual diameter 

JET 

Airbag = Parts 1 + 2 Jetting onto Part 2 

t 

fabric airbag 

(Part 1) 

These elements made 

rigid (part 2) 

A = Sum of spring forces 

B = Actual reaction force peak 

=> Factor = B/A 

Page 16.6


OASYS D3PLOT: AIRBAG WITH 30 DEGREE JETTING 




Z 

Y 

0.003997 

Z 

Y 

0.007998 

Z 

Y 

0.019997 

Z 

Y 

X 

X 

X 

X 

OASYS D3PLOT: AIRBAG WITHOUT JETTING 




Page 16.7 

Z 

Y 

0.003997 

Z 

Y 

0.007998 

Z 

Y 

0.019997 

Z 

Y 

X 

X 

X 

X


Pressure 

145 

140 

135 

130 

125 

120 

115 

110 

105 

E-3 

100 

0 0.02 0.04 0.06 0.08 0.10 

Time 

With Jetting 

Without Jetting 

MULTI-CHAMBER AIRBAGS 

AIRBAG WITH 30 DEGREE JETTING 

Oasys T/HIS Version 7.0 14-Apr-97 

Oasys T/HIS 

Version 7.0 

14-Apr-97 

Side-impact airbags frequently contain many separate chambers, with venting occurring between 

the chambers. These chambers can be modelled as separate airbags in LS-DYNA. Each airbag 

is given a unique ID at the end of the *AIRBAG keyword. The *AIRBAG_INTERACTION 

keyword is then used to define the amount of venting between each pair of adjacent chambers. 

The venting is based on a vent area and a shape factor and increases with the pressure difference 

between the chambers. The vent area can be defined explicitly as a constant, or via a load curve 

as a function of time by using a negative value whose absolute value is the load curve ID. 

Alternatively, a part ID can be given instead; in this case, the total area of all shell elements in 

this part is used for the vent area. The vent hole can then be meshed with shells made of a null 

material, and the part ID of these shells used for the vent area. Any change in size of the hole as 

the bag inflates will thus lead to changes in the mass flow rate between the chambers. 

*AIRBAG_SIMPLE_AIRBAG MODEL_1 

$ SET ID SET TYPE RIGID ID V FACTOR P FACTOR VOLUME DAMPING S FACT 

1 1 0 0.000E+00 0.000E+00 0.000E+00 5.000E+01 0.700E+00 

8.500E+08 1.100E+09 8.000E+02 1 1.000E+00 50.00000 1.019E-01 1.200E-12 

0 


1 

1 3 

$ 

Page 16.8


*AIRBAG_SIMPLE_AIRBAG MODEL_2 

$ SET ID SET TYPE RIGID ID V FACTOR P FACTOR VOLUME DAMPING S FACT 

2 1 0 0.000E+00 0.000E+00 0.000E+00 5.000E+01 0.700E+00 

8.500E+08 1.100E+09 8.000E+02 1 1.000E+00 50.00000 1.019E-01 1.200E-12 

0 


2 

2 3 

$ 

$ 

*AIRBAG_INTERACTION 

1 2 500 1.0 0 

ERRORS 

Two common errors in airbag simulations are: 

(I) Negative energy in control volume. This is usually caused by one of: 

! Fabric layers insufficiently widely spaced 

! Inconsistent units 

! Mass flow curve too high 

! Jet focus too close to airbag 

! Jet blowing the wrong way (which is visible in D3PLOT) 

! Contact errors 

! Timestep too big with folded mesh 

(ii) Negative mass in control volume. This is usually caused by a very large vent area leading 

to all the gas escaping in a single timestep. If such a large vent area is really required, 

reduce the timestep. 

Page 16.9


Page 16.10


17.0 SHEET METAL FORMING SIMULATIONS 

LS-DYNA has been used extensively for sheet metal forming simulation for many years. The 

solver includes many features specifically for simulating manufacture by draw die, although 

many other sheet metal processes such as tubular hydro forming, fluid cell forming, roll forming 

and superplastic forming can also be simulated. The goal in any such simulation is to confirm 

that the proposed manufacturing process will give a successful end result, thereby reducing press 

try out time and hence producing cost savings. An efficient modelling strategy is required to 

achieve an effective contribution to production operations. The following notes are intended to 

draw attention to some of the features of LS-DYNA which should be considered when setting 

up a draw die simulation. 

SEQUENCE OF OPERATIONS 

The complete sequence would be: 

` gravity wrap 

` blank holder closure or wrap 

` forming operation (stretch, draw, flange, etc) 

` trimming 

` springback 

Multiple draw operations can be simulated by looping this sequence. It is often preferable to 

conduct each of these phases as separate calculations with restarts used to move to the next 

phase; this allows parameters to be set up optimally for each operation. 

In previous versions of LS-DYNA, two options were available for calculating springback after 

forming; dynamic relaxation or output of a file for submission to LS-NIKE3D (using the 

*INTERFACE_SPRINGBACK keyword). These methods have now been superseded by the 

addition of the implicit solver options within LS-DYNA itself. The implicit mode can be 

activated in two ways. A simulation can be run entirely in implicit mode using the 

*CONTROL_IMPLICIT_GENERAL keyword; the input file for this can be automatically 

created by LS-DYNA at the end of the forming phase using the 

*INTERFACE_SPRINGBACK_DYNA3D keyword. Alternatively an explicit simulation may 

be seamlessly switched into implicit mode at a specific time using the 

*INTERFACE_SPRINGBACK_SEAMLESS keyword. Several other *CONTROL_IMPLICIT 

keywords have been added to LS-DYNA to control the implicit analysis; default values have 

been carefully selected to minimise user input. 

The implicit analysis capability within LS-DYNA also now allows it to be used for the gravity 

wrap and blankholder wrap stages of the forming sequence, allowing more efficient and more 

accurate calculation of these quasi-static stages. 

Page 17.1


Associated with springback is the *DATABASE_SPRING_FORWARD option to output a nodal 

force file used in an iterative approach to die correction for springback. 

Please contact Oasys for more information on LS-NIKE3D and its use in springback calculations. 

(Note that LS-NIKE3D may also be considered for simulating the blank holder warp stage of the 

process - this is still under development at LSTC). 

BLANK 

The undeformed blank should be meshed using shell elements as use of solids would be 

prohibitively costly due to the large number of elements and the small timestep required. The 

default B-T shell is generally acceptable but the number of integration points should be increased 

to five or more for increased accuracy in the springback calculation. Membrane elements can 

be used where cpu usage is critical but care must be exercised in interpreting the results. Wellconditioned 

quadrilateral elements are preferred as triangles and “chevron” elements can give 

local changes in stiffness. 

Element size in the blank should be as small as reasonable for the draw phase, although larger 

elements can be used in the gravity and blank holder wrap. Adaptive re-meshing is very helpful 

especially where there are tight radii in the tooling surfaces. If an element on the blank is too 

large at a tight radius excess, force will be developed leading to excess constraint or even a 

locked condition. Adaptivity allows the mesh to be refined locally only as required in the 

calculation and is more efficient than using a very fine uniform mesh. It is also much easier to 

prepare than a structured mesh manually refined in selected areas. The option to output the final 

adapted mesh without displacements is a useful way to carry out sensitivity analyses. The last 

version of LS-DYNA can adapt the mesh prior to contact with the tooling. This “look ahead” 

capability gives the most efficient and reliable implementation of adaptive remeshing (see the 

comments below on Control Cards for more details). 

In order to represent the elastic-plastic deformation of the blank, the standard material models 

applicable to shells may be used but there are also several models provided specifically for sheet 

metal forming simulation. The manufacturing process for sheet metal means that the material 

properties are no longer isotropic. Rolling introduces anisotropy in the through-thickness 

direction such that the ratio of width strain to thickness strain, r, is not unity. For most steel r > 

1 giving improved drawability. In addition, r can vary along or across the sheet leading to 

definition of r 00, r 45 and r 90 to attempt to represent the anisotropy in more detail; this is normally 

required to capture the behaviour of aluminium alloys. 

Anisotropy is included in a number of models. 

*MAT_TRANSVERSELY_ANISOTROPIC_ELASTIC_PLASTIC is based on Hill’s 1948 

quadratic yield surface taking into account normal anisotropy (the ‘r’ value); this model equates 

to Von Mises with r = 1. (*MAT_FLD_TRANSVERSELY_ANISOTROPIC is identical but 

includes definition of a forming limit diagram to calculate an additional parameter used in certain 

post-processors; Oasys D3PLOT does not require this variable). *MAT_3- 

PARAMETER_BARLAT is based on Barlat’s three parameter yield surface model using the 

planar anisotropy parameters r 0, r 45 and r 90 (a full implementation of Barlat is also available). 

This should always be used for aluminium (Hill should not be used in this case). One other 

Page 17.2


model of interest is *MAT_POWER_LAW_PLASTICITY which allows the commonly used 

parameters n & K to be used directly; these are often available from the material supplier, and 

n is critical in assessing the forming limit of the material. This model also includes strain rate 

sensitivity (but see discussion below on scaling tool velocity). As with all material models in LS- 

DYNA, work hardening data must always be based on true stress vs. true strain values. 

Generally, splits in a blank occur due to a strain limit defined in the plane of the sheet by a 

forming limit curve. It is most convenient to assess splitting by post-processing, comparing 

values with the forming limit curve (e.g in Oasys D3PLOT) rather than attempt to include failure 

in the analysis. 

TOOLS 

The tooling surfaces (punch, die, upper and lower rings, etc.) are usually represented by rigid 

elements, typically shells, although in some cases where flexibility of the blank holder ring is 

important it is worth considering modelling the ring with elastic solids (with obvious cpu 

penalties); Rigid to Deformable switching can sometimes be useful here. The rules on mesh 

generation for tool surfaces are more flexible than for deformable parts; the mesh does not have 

to be continuous and can use high aspect ratio elements for example, but this may put excessive 

demands on the contact surface. It is important, however, that the intended geometry is 

accurately represented. Small radii require small elements and at least five elements around a 

90b radius are recommended. Automatic mesh generation techniques that modify the element 

size according to the geometry are very useful for creating tool models; eta\DYNAFORM has 

a powerful tool mesh generator. 

LS-DYNA offers the option to use CAD data directly to represent the tools; both IGES and VDA 

databases are supported. The VDA option has generally been the most effective mostly because 

of the wide variation in IGES definitions. Use of CAD data gives the most accurate 

representation of the tooling surfaces as no discretisation of the geometry is required (a coarse 

mesh is generated automatically for ease of post-processing - this is not used in the calculation). 

Springback prediction will also be improved as stresses are more accurate. This option offers 

significant time savings in model creation but does require high quality, fully trimmed surface 

definition with no overlaps and very small gaps. It is also often more demanding on cpu. The 

file containing the location CAD data must be identified in the Oasys submission shell; an alias 

must be defined on each *PART card to identify which file is the die, which the punch etc. 

Options in LS-DYNA associated with use of CAD data include the ability to translate the surface 

to its initial position and a function to create one tool from another by a normal offset. 

Implementation is by means of aliases on each *MAT_RIGID card together with a file 

identifying which surfaces are associated with which alias (this file can be specified using the 

Additional Files option in the Oasys submission shell). The syntax for this file is given in the 

user manual; see Appendix I for more details. 

TOOL MOTION 

Page 17.3


In some cases it is necessary to commence the forming analysis by calculating the sag of the 

blank under self-weight when placed on the blankholder. This sag allows extra material into the 

die cavity which can make a difference to part formability. *LOAD_BODY keywords together 

with *DAMPING_GLOBAL can be used to simulate the effects of gravity. This may be 

calculated more accurately using the implicit options. 

As far as possible, the motion of the simulated tools should reflect those in the real press. It is 

useful to orient the model such that the motion is all in the global z direction. One tool is 

typically fixed while the others are limited to movement in z only, using the rigid body constraint 

options on the *MAT_RIGID card. 

The tools should be positioned initially as close as possible to minimise wasted cpu while 

moving the tool through “fresh air”. Care should be taken that the action of one tool will not 

cause the blank to move towards another in an unexpected way - i.e., keep the punch clear during 

the blank holder wrap. 

In a mechanical press the displacement of the upper tool is controlled by a flywheel. The same 

set up is adopted in the analysis - i.e. the motion of the upper tool is defined using a 

*BOUNDARY_PRESCRIBED_MOTION_RIGID card. The associated load curve, usually in 

terms of a velocity, will move the tool towards the blank slowly, accelerate to a plateau and then 

often reduce to zero at the end. It is desirable to have lower velocities when rigid tools first 

contact the deformable blank. The maximum velocity of a real press may be of the order 0.1 m/s; 

using this velocity in the analysis would lead to unacceptable run times so the velocity is 

increased by anything from 10x to 100x in the analysis (A maximum velocity of 2m/s for the 

blankholder closure and 5m/s for the draw is recommended). Loads and velocities should be 

ramped and never changed instantaneously. The user must beware of dynamic effects introduced 

by this increase in speed; the ratio of internal to kinetic energy in the blank (KE


DRAWBEADS 

The drawbead is an important feature of draw die operations to control the motion of the blank 

into the die cavity. They can be included in a LS-DYNA model in a number of ways. The most 

accurate approach is to include the bead geometry as part of the tooling mesh. In this way, not 

only the action perpendicular to the bead is represented but also parallel motion and end effects. 

The material is not only restrained but also strained giving more accurate thinning predictions 

near the bead and work hardening of the blank material. Unfortunately, draw beads can have 

very small radii (


There are many ways to handle thickness in contact. The old algorithms (i.e, those using node 

based contact searching) exclude thickness but are not recommended. The old types 3, 5 & 10 

can be made to include thickness for the blank only or for both blank and tools; and the new 

automatic routines (using segment searching) will always include thickness. However, the 

thickness used in either slave or master side can be scaled or re-defined on the *CONTACT_ 

card as required and is also affected by flags on the *CONTROL_CONTACT card (which can 

also be over ruled by Optional Card B). Which option used depends on how the upper and lower 

tools are defined (whether they are offset from each other, which surface of the tool they 

represent, etc.). This issue must be handled carefully as an error can cause unrealistic splits due 

to trapped material. 

The default algorithm generally recommended for forming simulation is *CONTACT- 

FORMING_ONE-WAY_SURFACE_TO_SURFACE. This is a fast algorithm that can cope 

with discontinuities in the tool mesh. Blank thickness should be included but the tool thickness 

is generally ignored (by setting shlthk = 1 on *CONTROL_CONTACT). However, the tools can 

be offset by specifying a negative value of thickness in the *CONTACT card. This is very useful 

if the punch and die are not offset in the CAD data. Alternatively, many pre-processors (e.g. 

eta/DYNAFORM) can offset a mesh by a specified normal direction to achieve the same result. 

Friction between tool and blank is specified by setting the Coulomb coefficient on the 

*CONTACT card. Typical metal to metal contact would be represented by a value of fs ³ 0.15 

(higher for aluminium blanks). A lower value would be used if lubrication was being employed. 

More complex relationships between the friction coefficient and relative velocity and/or pressure 

can be implemented, if suitable data is available by setting fs = 2 and using *DEFINE_TABLE. 

User defined subroutines can also be set up. 

A useful option to consider with penalty based contact methods is contact damping; this can help 

reduce the oscillations when tool and blank contact at speed and gives improved prediction of 

punch force. The value to be entered is a percentage; 20 is a typical value. 

The *CONTACT_ENTITY card must be used if the IGES or VDA options are used. 

Constraint types of contact can be used in sheet metal forming, but can only be used on one side 

of the blank. 

TRIMMING 

LS-DYNA includes an algorithm to trim material from the blank (and re-mesh to a specified 

trim line). This has been implemented chiefly for a more realistic springback calculation (as the 

trimming material can relieve stresses, significantly affecting the results) but can also be used as 

part of a multistage forming operation. Note that this is not a simulation of the physical trimming 

process but simply a procedure to delete elements and nodes in the region to be trimmed. Where 

the trim line passes through an element, that element is adapted, according to a tolerance set by 

the user. A tighter tolerance will more accurately follow the trim curve but will produce smaller 

elements. 

Page 17.6


The trimming option is set up using the *DEFINE_CURVE_TRIM option. The trim data can 

be either x,y data points (projected into the correct plane using a *DEFINE_VECTOR card as 

necessary) or IGES or VDA data contained in a file. An arbitrary number of trim curves may be 

specified as long as curves do not intersect and each element is trimmed by only one curve. 

Curves may extend outside the part to be trimmed but LS-DYNA always treats a curve as a 

closed loop. Material can be removed either inside or outside the specified line. Note that pretrimming 

is also possible using this option by specifying a *ELEMENT_TRIM card; if this card 

is not in the deck then trimming occurs at the end of the run. A special procedure is required to 

trim an adaptive mesh - see the *INTERFACE_SPRINGBACK card for details. 

A users guide to adaptive mesh trimming is available; please contact Oasys for more details. 

Alternatively, dedicated metal forming pre-processors, such as eta/DYNAFORM, are often 

capable of trimming a model. 

CONTROL CARDS 

Certain control card options are suggested for sheet metal forming. 

The *CONTROL_SHELL card includes a flag called istupd; this should be set to 1 so that 

membrane strains in shells cause thickness changes which is important for sheet metal forming 

simulation. 

The penalty stiffness value and the thickness flags (including shlthk and ssthk) on the 

*CONTROL_CONTACT card interact with the contact definitions and should be checked 

carefully. If a non-continuous mesh is used for the tools it may be necessary to increase the 

bucket search frequency. 

Scaling the tool velocities has been mentioned. It is also possible to speed up the analysis using 

the mass scaling options, with the same caveats about dynamic effects. At the simplest level, 

mass scaling can be implemented by simply increasing the density of the blank material. 

However, the *CONTROL_TIMESTEP card allows a minimum time step to be maintained by 

setting dt2ms = negative value of desired timestep (be aware of the mass increase termination 

option set on the *CONTROL_TERMINATION card). Mass scaling is easier to implement than 

velocity scaling as only one value has to be changed. In practice, “a bit of both” is used, with 

modest levels of velocity scaling combined with mass scaling adjusted to check for dynamic 

effects. 

Adaptive remeshing has already been mentioned and is defined using the 

*CONTROL_ADAPTIVE card (and do not forget to set the appropriate flag on the *PART card 

for the blank). A tolerance of 5 degrees and three levels of adaptivity are good starting options. 

Previously, the more expensive, option to repeat the previous cycle after adaption (adpass=0) 

was advisable otherwise new nodes created by adaptivity could be on the “wrong” side of the 

contact surface. The latest version of LS-DYNA allows adaptivity to take place before contact 

between blank and tool takes place. This is achieved by setting adpene to a positive value. The 

Page 17.7


contact search will then identify where contact to the tooling will occur and will adapt the blank 

mesh according to the curvature of the tooling. Although this can create somewhat more 

elements than the two pass option it does allow the single pass option to be used (adpass = 1) 

giving the most efficient result. This option works best with the _FORMING_ contact algorithm; 

it also requires a fairly frequent check (adpfreq should be set so that the tools move less than the 

value of adpene between adaptions). Adaptivity can be turned on and off during the analysis to 

reduce the additional cpu demand. The ioflag is useful to obtain the adapted mesh (with no 

displacements) at the end of the run. Mass scaling is generally used to prevent the small elements 

created by adaptivity from controlling the timestep. 

Metal forming is well suited to parallel processing and excellent speed up factors can be obtained 

with LS-DYNA. The number of processors to be used is set using *CONTROL_CPU. 

DATABASE CARDS 

It is essential that the strain tensor is included in the output; set the variable strflg to 1 on the 

*DATABASE_EXTENT_BINARY card. The compressed database option is worth considering 

as it will greatly reduce the size of the d3plot files because it will omit superfluous data relating 

to the rigid tooling. 

POST-PROCESSING 

Almost all of the useful data from a sheet metal forming simulation is in terms of strains; total 

plastic strain is insufficient to assess the success or failure of the process and even thickness 

strains do not, on their own, give an assessment of the likelihood of splitting. The strain tensor, 

projected into the plane of the blank, gives us the major and minor strains. These strains can be 

plotted on a Forming Limit Diagram and compared with the Forming Limit Curve for that 

material (for low carbon steels this can be estimated from the material thickness and n value; for 

other materials experimental data must be obtained). This diagram is used to indicate splits and 

contour plots of formability can be derived from this. Oasys D3PLOT allows display of the FLD 

and formability contours with the option to click on a point in the FLD to turn on the 

corresponding element label on the contour plot. 

The direction of major and minor strains is also very helpful to understand material flow. Strain 

paths for selected elements should also be checked to help understand the forming process. 

These and several other types of data (thickness value, thickness strain, blank edge movement, 

wrinkle visualisation using shading plus links to ray-tracing packages, for highly accurate 

visualisation of surface deflects etc.) can be viewed using Oasys D3PLOT. Strains are generally 

in true values, but can be plotted as engineering strains (in %) for FLD plotting. Oasys D3PLOT 

also includes a DIE-CLOSURE plot which calculates the distance of the blank to a selected tool 

or tools; this is very useful for checking for complete tool closure and for die filling in 

hydroforming simulations. 

KEYWORDS USED IN METAL FORMING 

Page 17.8


` AIRBAG - pressure in hydro forming 

` BOUNDARY_PRESCRIBED_MOTION_RIGID 

` CONSTRAINED_RIGID_BODY_STOPPERS 

` CONSTRAINED_EXTRA_NODES_OPTION (drawbeads) 

` CONTACT 

` CONTACT_ENTITY (VDA or IGES data) 

` CONTROL (implicit, adaptivity) 

` DAMPING 

` DATABASE 

` DEFINE (i.c., box, co-ords, vectors etc) 

` DEFORMABLE_TO_RIGID (def of tooling) 

` ELEMENT 

` INCLUDE 

` INITIAL (esp stresses and strains) 

` INTERFACE 

` LOAD (pt load, pressure, gravity) 

` MAT 

` NODE 

` PART 

` SECTION 

` SET 

` TERMINATION (stop due to displacement or contact force) 

` TITLE 

Page 17.9


Page 17.10


Introduction 

Appendix A 

Keyword Input Deck Examples 

This Appendix contains a number of example keyword input decks to give the user the idea of 

a keyword input deck. In some cases sections of the input decks have been removed to reduce 

the amount of repetition. All of these examples can be found on in the directory examples_dir 

(examples on Windows NT) supplied with the LS-DYNA installation. 

The resources and histories are documented in the acknowledgment and reference sections. 

Users are encouraged to submit examples which will facilitate the education of LS-DYNA users. 

. 

Page A.1


Page A.2


LS-DYNA Manual Section: *AIRBAG_SIMPLE_AIRBAG_MODEL 

Additional Sections: *CONTACT_NODES_TO_SURFACE 

Example of: Airbag Deploys into Cylinder 

Example Filename: airbag_deploy.key 

Description: 

An airbag inflates an contacts an adjacent rigid cylinder. 

Model: 

The volume pressure relationship for the airbag is defined using the Simple Airbag Model for 

control volumes. The bag inflates through the flow of mass into the bag. The termination time 

is 0.01 seconds. 

Input: 

The control volume defines the thermodynamic relationship for the gas in terms of parameters such 

as heat capacity, gas temperature, incoming mass, and outgoing mass 

(*AIRBAG_SIMPLE_AIRBAG_MODEL). The contact surfaces are automatically generated using 

part id’s(*CONTACT_NODES_TO_SURFACE). 

Results: 

The plots show the expaned airbag at the end of the analysis and the pressure time history for the 

airbag that has been extracted from the XTF file. 

Page A.3


List of LS-DYNA input deck: 

*KEYWORD 

*TITLE 

AIRBAG AND STRUCTURE 

$ 

$================================ CONTROL CARDS ================================ 

$ 


$ [1] Termination time [2] Termination Cycle [3] Minimum timestep scale factor 

$ [4] % Energy change for termination [5] % Mass change for termination 

$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ] 

1.000E-02 0 .000E+00 .000E+00 .000E+00 

*CONTROL_SHELL 

$ [1] Shell warpage angle [2] Automatic sorting of triangles [3] Hughes-Liu 

$ update option [4] Shell thickness change option [5] Shell theory [6] Warping 

$ stiffness [7] Plane stress plasticity option 

$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 0 0 0 0 0 0 


$ [1] Interface penalty scale factor [2] Rigid wall penalty scale factor 

$ [3] Initial penetration check [4] Shell thickness in type 3,5,10 contacts [5] 

$ Penalty stiffness option [6] Consider shell thickness change (single surface 

$ contact) [7] Automatic reorientation of interface segments 

$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 .000E+00 0 0 1 0 0 

$ [1] Storage per contact surface [2] Storage per user defined friction 

$ [3] Timesteps between bucket searches [4] Intermittent searching [5] Search 

$ multiplier [6] Shell thickness logic [7] Timstep override for eroding contacts 

$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

0 0 0 0 .000E+00 

*CONTROL_ENERGY 

$ [1] Compute hourglass energy [2] Compute stonewall energy dissipation 

$ [3] Compute sliding interface energy [4] Compute Rayleigh energy dissipation 

$ 1 ][ 2 ][ 3 ][ 4 ] 

0 0 0 0 

*CONTROL_DAMPING 

$ [1] No cycles between convergence checks [2] DR convergence tolerance [3] DR 

$ damping factor [4] DR Optional termination time [5] Scale factor for DR time 

$ step [6] Automatic control for DR option [7] Convergence tolerance for 

$ automatic DR [8] DR flag for stress initialization 

$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ][ 8 ] 

0 .000E+00 .000E+00 .000E+00 .000E+00 0 .000E+00 0 


$ [1] Print suppression during input phase [2] Print suppression for echo file 

$ [3] Update beam reference nodes [4] Average accelerations from velocities 

$ [5] Output interval for interface file [6] Print all element initial timestep 

$ [7] Number of cycles between output to otf file 

$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

0 0 0 0 .000E+00 0 0 

*CONTROL_TIMESTEP 

$ [1] Initial timestep size [2] Scale factor for computed timestep [3] Basis of 

$ timestep size calculation [4] Minimum timestep for shell elements [5] Timestep 

$ size for mass scaled solution [6] Load curve number that limits time step 

$ [7] Erode solids and shells when minimum timestep reached 

$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 .000E+00 0 .000E+00 .000E+00 0 0 0 

$ 

$================================ DATABASE CARDS =============================== 

$ 

*DATABASE_ABSTAT 

2.000E-04 

*DATABASE_BINARY_D3PLOT 

2.000E-04 0 1 

*DATABASE_BINARY_XTFILE 

*DATABASE_BINARY_D3THDT 

.000E+00 0 

*DATABASE_BINARY_D3DUMP 

0 

*DATABASE_BINARY_RUNRSF 

0 

*DATABASE_BINARY_INTFOR 

2.000E-04 0 

*DATABASE_EXTENT_BINARY 

0 0 0 0 0 0 0 0 

0 0 0 

$ 

$============================ MATERIAL PROPERTIES ============================== 

$ 

Page A.4


*MAT_ELASTIC 

$ Material 1 : PLATE - ELASTIC 

1 7.840E-04 3.000E+07 .3000 .000E+00 .000E+00 

$------------------------------------------------------------------------------- 

*MAT_ELASTIC 

$ Material 2 : CYLINDER - RIGID 

2 7.840E-04 3.000E+07 .3000 .000E+00 .000E+00 

$------------------------------------------------------------------------------- 

*MAT_FABRIC 

$ Material 3 : AIRBAG - FABRIC 

3 1.000E-04 2.000E+06 2.000E+06 2.000E+06 .3500 .3500 .3500 

1.530E+06 1.530E+06 1.530E+06 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 

.0 

.000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 

.000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 

$ 

$============================= SECTION PROPERTIES ============================== 

$ 


$ Section 1 : PLATE - ELASTIC 

1 0 .00000 .0 .0 .0 0 

5.000E-01 5.000E-01 5.000E-01 5.000E-01 .000E+00 

$------------------------------------------------------------------------------- 


$ Section 2 : AIRBAG - FABRIC 

2 9 .00000 4.0 .0 .0 1 

1.500E-02 1.500E-02 1.500E-02 1.500E-02 .000E+00 

.000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 

$ 

$============================== PART DEFINITIONS =============================== 

$ 

*PART 

PLATE - ELASTIC 

1 1 1 0 0 0 

$------------------------------------------------------------------------------- 

*PART 

CYLINDER - RIGID 

2 1 2 0 0 0 

$------------------------------------------------------------------------------- 

*PART 

AIRBAG - FABRIC 

3 2 3 0 0 0 

$ 

$=================================== NODES ===================================== 

$ 

*NODE 

$ ID X COORDINATE Y COORDINATE Z COORDINATE TRANS ROT 

1 -.12000000E+02 .00000000E+00 -.13000000E+02 0 0 

... 7147 .10500000E+02 .15000001E+00 .12500000E+02 0 0 

$ 

$================================== ELEMENTS =================================== 

$ 


$ ID PART NODE 1 NODE 2 NODE 3 NODE 4 

1 1 1 62 63 2 

... 6992 3 5998 7108 7146 7147 

$ 

$============================ BOUNDARY CONDITIONS ============================== 

$ 

*BOUNDARY_SPC_NODE 

$ NODE COORD-SYS X-TRANS Y-TRANS Z-TRANS X-ROT Y-ROT Z-ROT 

1 1 1 1 1 1 1 1 

... 

3721 1 1 1 1 1 1 1 

*DEFINE_COORDINATE_SYSTEM 

1 .0 .0 .0 1.0 .0 .0 

.0 1.0 .0 

$ 

$================================= CONSTRAINTS ================================= 

$ 

$ 

$================================= RIGID WALLS ================================= 

$ 

$ 

$============================== INITIAL CONDITIONS ============================= 

$ 

$ 

$================================== LOADING ==================================== 

$ 

Page A.5


$ 

$============================== CONTACT SURFACES =============================== 

$ 

*CONTACT_NODES_TO_SURFACE_TITLE 

$ NUMBER NAME 

1 Contact # 1 

$ SL SET MA SET SL TYPE MA TYPE SL BOX MA BOX PRINT SL PRINT MA 

1 2 2 2 0 0 1 1 

$ STATIC DYNAMIC DECAY VISCOUS VIS DAMP PENCHK BIRTH DEATH 

5.000E-01 5.000E-01 .000E+00 .000E+00 .000E+00 0 .000E+00 .000E+00 

$ SL FACT MA FACT SL THICK MA THICK SL T-FACT MA T-FACT COULOMB VISCOUS 

1.000E+00 6.700E-02 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 

$ SOFT OPT FACTOR LC THICK MAXPAR PENTOL DEPTH SORT FREQ 

0 .000E+00 0 .000E+00 .000E+00 0 0 0 

$ MAX PEN THKOPT SHLTHK SNLOG 

.000E+00 0 0 

*SET_PART 13 

*SET_PART 21 

$------------------------------------------------------------------------------- 


$ NUMBER NAME 

2 Contact # 2 


3 4 2 2 0 0 1 1 


5.000E-01 5.000E-01 .000E+00 .000E+00 .000E+00 0 .000E+00 .000E+00 


1.000E+00 6.700E-02 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 


0 .000E+00 0 .000E+00 .000E+00 0 0 0 


.000E+00 0 0 

*SET_PART 33 

*SET_PART 42 

$ 

$=============================== LOAD CURVES =================================== 

$ 

*DEFINE_CURVE 

$ CURVE ID X FACTOR Y FACTOR X OFFSET Y OFFSET 

1 0 .000E+00 .000E+00 .000E+00 .000E+00 

.00000000E+00 .00000000E+00 

.32000002E-01 .26000000E+02 

.45000002E-01 .60000002E+00 

.79999998E-01 .10000000E+00 

$ 

$=================================== AIRBAGS =================================== 

$ 

*AIRBAG_SIMPLE_AIRBAG_MODEL 

$ SET ID SET TYPE RIGID ID V FACTOR P FACTOR VOLUME DAMPING S FACTOR 

5 1 0 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 

1.736E+03 2.430E+03 1.200E+03 1 7.000E-01 .000E+00 1.470E+01 3.821E-06 

0 

*SET_PART 53 

*END 

Page A.6


Results: 

OASYS D3PLOT: AIRBAG AND STRUCTURE 

Pressure 

50 

45 

40 

35 

30 

25 

20 

15 

10 

Z 

Y 

.010000 

0 2 4 6 8 10 

E-3 

Time 

Pressure - c. vol. 1 

AIRBAG AND STRUCTURE 

Oasys T/HIS Version 7.0 4-Feb-97 


Version 7.0 

4-Feb-97 

X 

Page A.7


LS-DYNA Manual Section: *CONSTRAINED_JOINT_PLANAR 

Additional Sections: *LOAD_NODE_POINT 

*LOAD_SEGMENT 

*INITIAL_VELOCITY 

*CONSTRAINED_NODES_EXTRA_SET 

Example of: Sliding Blocks with Planar Joint 

Example File Name: joint_planar.key 

Description: 

This problem illustrates a planar joint connecting two rigid bodies. 

Model: 

The first block measuring 2 × 2 × 2 slides along a second block measuring 2 × 2 × 8. A third 

flexible body controls the time step size. The first block has a ramped pressure of 100 psi applied 

to the top surface and ramped concentrated nodal forces applied to a lower edge of 40 lbs. The 

initial velocity of the first block is 400 inches/second. 

Input: 

The model contains a single joint definition consisting of nodes 128, 126, 129 and 127 

(*CONSTRAINED_JOINT_PLANAR). These nodes are coincident and are attached to the rigid 

bodies as extra nodes (*CONSTRAINED_EXTRA_NODES_SET, *SET_NODE_LIST) 

Results: 

The plots simply show that the first block correctly slides across the second block. 

Page A.8



*KEYWORD 

*TITLE 

LINEAR CONSTRAINT EQUATIONS 

$ 

$================================ CONTROL CARDS ================================ 

$ 




$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ] 

5.000E-04 0 .000E+00 .000E+00 .000E+00 





$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

2.000E+01 2 -1 0 1 2 1 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

1.000E-01 .000E+00 2 0 1 0 0 




$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

0 0 0 0 .000E+00 




$ 1 ][ 2 ][ 3 ][ 4 ] 

0 0 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ][ 8 ] 

0 .000E+00 .000E+00 .000E+00 .000E+00 0 .000E+00 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

0 0 0 0 .000E+00 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 .000E+00 0 .000E+00 .000E+00 0 0 0 


4 .000E+00 

$ 


$ 


2.000E-05 0 1 



1.000E-06 0 


0 


0 


2.000E-05 0 


0 0 0 1 0 0 0 0 

0 0 0 

$ 


$ 

Page A.9


*MAT_ELASTIC 

$ Material 1 : IMPACTED MATERIAL 

1 2.000E-08 1.000E+05 .3000 .000E+00 .000E+00 

$ 


$ 


$ Section 1 : IMPACTED MATERIAL 

1 6 .83330 2.0 3.0 .0 0 

2.000E+00 2.000E+00 2.000E+00 2.000E+00 .000E+00 

$ 


$ 

*PART 

IMPACTED MATERIAL 

1 1 1 0 0 0 

$ 

$=================================== NODES ===================================== 

$ 

*NODE 


1 .00000000E+00 .00000000E+00 .00000000E+00 0 0 

... 

81 .40000000E+02 .40000000E+02 .00000000E+00 0 0 

$ 

$================================== ELEMENTS =================================== 

$ 



1 1 1 2 11 10 

... 

64 1 71 72 81 80 

$ 


$ 



1 1 0 0 1 0 0 0 

... 

81 1 0 0 1 0 0 0 


1 .0 .0 .0 1.0 .0 .0 

.0 1.0 .0 

*BOUNDARY_PRESCRIBED_MOTION_NODE 

$ NODE ID DOF TYPE CURVE ID FACTOR VECT ID 

41 3 2 1 1.000E+00 0 .000E+00 

$ 

$================================= CONSTRAINTS ================================= 

$ 

*CONSTRAINED_LINEAR 

$ NUM 2 

$ NODE ID DOF X DOF Y DOF Z DOF RX DOF RY DOF RZ COEFF 

40 1 1.00 

42 1 -1.00 

$ 


$ 

$ 


$ 

$ 

$================================== LOADING ==================================== 

$ 

$ 

$=============================== LOAD CURVES =================================== 

$ 

*DEFINE_CURVE 


1 0 .000E+00 .000E+00 .000E+00 .000E+00 

.00000000E+00 .00000000E+00 

.50000002E-03 -.15000000E+02 

*END 

Page A.10


Results: 

OASYS D3PLOT: TEST PLANAR JOINTS 

OASYS D3PLOT: TEST PLANAR JOINTS 

Deformable body for timestep control 

Joint 

Z 

Y 

X 

.000000000 

Z 

Y 

.019993 

X 

Page A.11


LS-DYNA Manual Section: *CONSTRAINED_LINEAR 

Example of: Linearly Constrained Plate 

Example Filename: plates_constrained.key 

Description: 

The center node of a plate moves in the direction normal to the plate. Two other nodes that are 

neighbors to the center node are constrained such that their displacement in the normal direction is 

identical. 

Model: 

The plate is made of an elastic material measuring 40 × 40 × 2 mm 3 and contains 64 Hughes-Liu 

shell elements. The center node displacement increases linearly. At the termination time, 0.0005 

seconds, the displacement is 15 mm. 

The degree of freedom in the z-direction for the two constrained nodes is identical. 

Input: 

A load curve defines the magnitude of the prescribed displacement of the center node, 41 

(*BOUNDARY_PRESCRIBED_MOTION_NODE, *DEFINE_CURVE). 

A linear constraint card defines the coupling of the displacement in the z-direction between the two 

constrained nodes, 40 & 42, (*CONSTRAINED_LINEAR). Two equal coefficients with opposite 

signs control the displacement. 

Results: 

The plots simply show that the two constrained nodes displace the same amount. 

Reference: 

Schweizerhof, K. and Weimer, K. 

Page A.12



*KEYWORD 

*TITLE 

TEST PLANAR JOINTS 

$ 

$================================ CONTROL CARDS ================================ 

$ 

*CONTROL_STRUCTURED 




$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ] 

2.000E-02 0 .000E+00 .000E+00 .000E+00 





$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 0 0 0 0 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 .000E+00 0 0 1 0 0 




$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

0 0 0 0 .000E+00 




$ 1 ][ 2 ][ 3 ][ 4 ] 

0 0 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ][ 8 ] 

0 .000E+00 .000E+00 .000E+00 .000E+00 0 .000E+00 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

0 0 0 0 .000E+00 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 .000E+00 0 .000E+00 .000E+00 0 0 0 

$ 


$ 

*DATABASE_JNTFORC 

1.000E-05 


3.333E-05 0 1 



.000E+00 0 


0 


0 


3.333E-05 0 


0 0 0 0 0 0 0 0 

0 0 0 

$ 


Page A.13


$ 

*MAT_RIGID 

$ Material 1 : FIXED RIGID BODY 

1 7.850E-04 3.000E+07 .3000 .0 .0 .0 

1.0 7.0 7.0 

.000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 

$------------------------------------------------------------------------------- 

*MAT_RIGID 

$ Material 2 : SLIDING RIGID BODY 

2 7.850E-04 3.000E+07 .3000 .0 .0 .0 

.0 .0 .0 

.000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 

$------------------------------------------------------------------------------- 

*MAT_ELASTIC 

$ Material 3 : ELASTIC BODY FOR TIME STEP CONTROL 

3 7.850E-04 3.000E+07 .3000 .000E+00 .000E+00 

$ 


$ 


$ Section 1 : FIXED RIGID BODY 

1 0 

$------------------------------------------------------------------------------- 


$ Section 2 : SLIDING RIGID BODY 

2 0 

$------------------------------------------------------------------------------- 


$ Section 3 : ELASTIC BODY FOR TIME STEP CONTROL 

3 0 

$ 


$ 

*PART 

FIXED RIGID BODY 

1 1 1 0 0 0 

$------------------------------------------------------------------------------- 

*PART 

SLIDING RIGID BODY 

2 2 2 0 0 0 

$------------------------------------------------------------------------------- 

*PART 

ELASTIC BODY FOR TIME STEP CONTROL 

3 3 3 0 0 0 

$ 

$=================================== NODES ===================================== 

$ 

*NODE 


1 .00000000E+00 .00000000E+00 .00000000E+00 0 0 

... 

129 .10000000E+02 .40000000E+01 .10000000E+01 0 0 

$ 

$================================== ELEMENTS =================================== 

$ 


$ ID PART NODE 1 NODE 2 NODE 3 NODE 4 NODE 5 NODE 6 NODE 7 NODE 8 

1 1 1 2 12 11 31 32 42 41 

... 

45 3 118 119 121 120 122 123 125 124 

$ 


$ 

$ 

$================================= CONSTRAINTS ================================= 

$ 

*CONSTRAINED_EXTRA_NODES_SET 

$ PART ID NODE SET 

1 1 

*SET_NODE_LIST 

1 

126 127 



2 2 


2 

128 129 

*CONSTRAINED_JOINT_PLANAR 

$ NODE 1 NODE 2 NODE 3 NODE 4 NODE 5 NODE 6 STIFFNESS 

128 126 129 127 0 0 .000E+00 

Page A.14


$ 


$ 

$ 


$ 

*INITIAL_VELOCITY_NODE 

1 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 

... 

90 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 

91 4.000E+02 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 

... 

117 4.000E+02 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 

118 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 

... 

127 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 

128 4.000E+02 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 

129 4.000E+02 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 

$ 

$================================== LOADING ==================================== 

$ 

$ NODE DOF CURVE ID FACTOR CID M1 M2 M3 

*LOAD_NODE_POINT 

91 3 2-1.000E+00 0 0 0 0 

92 3 2-1.000E+00 0 0 0 0 

93 3 2-1.000E+00 0 0 0 0 

*LOAD_SEGMENT 

$ CURVE ID FACTOR TIME NODE 1 NODE 2 NODE 3 NODE 4 

1 1.000E+00 .000E+00 97 106 107 98 

1 1.000E+00 .000E+00 106 115 116 107 

1 1.000E+00 .000E+00 98 107 108 99 

1 1.000E+00 .000E+00 107 116 117 108 

$ 

$=============================== LOAD CURVES =================================== 

$ 

*DEFINE_CURVE 


1 0 .000E+00 .000E+00 .000E+00 .000E+00 

.00000000E+00 .00000000E+00 

.99999998E-02 .10000000E+03 

.20000000E-01 .10000000E+03 

*DEFINE_CURVE 


2 0 .000E+00 .000E+00 .000E+00 .000E+00 

.00000000E+00 .00000000E+00 

.20000000E-01 .40000000E+02 

*END 

Page A.15


Results: 

OASYS D3PLOT: LINEAR CONSTRAINT EQUATIONS 

OASYS D3PLOT: LINEAR CONSTRAINT EQUATIONS 

N40 N41 N42 

N40 

N41 

N42 

Y 

Z 

X 

.000000000 

Y 

Z 

.000499 

X 

Page A.16


LS-DYNA Manual Section: *CONSTRAINED_SHELL_TO_SOLID 

Example of: Impulsively Loaded Cap with Shells and Solids 

Example Filename: dome_shell-brick.key 

Description: 

A dome is subjected to an impulsive pressure load. The dome contains shell and brick element 

joined with shell-brick interfaces. 

Model: 

The dome shells are Hughes-Liu shell elements with three integration point through the thickness. 

Four shell elements have a pressure load of 5,308 psi over 0.0017246 square inches. The 

termination time is 0.0004 seconds. 

Input: 

The model contains seven shell-brick interfaces each containing 1 shell node tied to 5 brick nodes 

(*CONSTRAINED_SHELL_TO_SOLID). The model contains four pressure surfaces 

(*LOAD_SEGMENT). Four nodes are written to the time history binary database every 3 µsec 

(*DATABASE_HISTORY_NODE, *DATABASE_D3THDT). 

Results: 

The plots show the response of the dome. 

Reference: 

T. Littlewood 

Page A.17



*KEYWORD 

*TITLE 

EXAMPLE OF SHELL BRICK INTERFACES 

$ 

$================================ CONTROL CARDS ================================ 

$ 




$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ] 

4.000E-04 0 .000E+00 .000E+00 .000E+00 





$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 0 0 0 0 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 .000E+00 0 0 1 0 0 




$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

0 0 0 0 .000E+00 




$ 1 ][ 2 ][ 3 ][ 4 ] 

0 0 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ][ 8 ] 

0 .000E+00 .000E+00 .000E+00 .000E+00 0 .000E+00 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

0 1000 0 0 .000E+00 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 .000E+00 0 .000E+00 .000E+00 0 0 0 

$ 


$ 

*DATABASE_GLSTAT 

5.000E-07 


5.000E-05 0 1 



3.000E-06 0 


0 


0 


5.000E-05 0 

*DATABASE_HISTORY_NODE 

1 116 284 361 326 

*DATABASE_HISTORY_SOLID 

1 

*DATABASE_HISTORY_SHELL 

1 

Page A.18



0 0 0 1 0 0 0 0 

0 0 0 

$ 


$ 

*MAT_ELASTIC 

$ Material 1 : BRICK -STEEL 

1 2.000E-04 2.900E+07 .3300 .000E+00 .000E+00 

$ 


$ 


$ Section 1 : BRICK -STEEL 

1 0 

$------------------------------------------------------------------------------- 


$ Section 2 : SHELL -STEEL 

2 0 .00000 .0 .0 .0 0 

1.576E-02 1.576E-02 1.576E-02 1.576E-02 .000E+00 

$ 


$ 

*PART 

BRICK -STEEL 

1 1 1 0 0 0 

$------------------------------------------------------------------------------- 

*PART 

BRICK 2 -STEEL 

2 1 1 0 0 0 

$------------------------------------------------------------------------------- 

*PART 

SHELL -STEEL 

3 2 1 0 0 0 

$ 

$=================================== NODES ===================================== 

$ 

*NODE 


1 .00000000E+00 .00000000E+00 .47915201E+01 0 0 

... 402 .00000000E+00 .90158439E+00 .46818609E+01 0 0 

$ 

$================================== ELEMENTS =================================== 

$ 



1 1 1 3 4 2 24 26 27 25 

... 204 2 282 283 46 45 324 325 23 22 



1 3 326 333 334 327 

... 

60 3 394 401 402 395 

$ 


$ 



1 1 1 1 0 1 1 1 

... 

402 1 1 1 1 1 1 1 


1 .0 .0 .0 1.0 .0 .0 

.0 1.0 .0 

$ 

$================================= CONSTRAINTS ================================= 

$ 

*CONSTRAINED_SHELL_TO_SOLID 

$ SHELL ID NODE SET 

326 1 


1 

116 158 200 242 284 



327 2 


2 

117 159 201 243 285 

Page A.19




328 3 


3 

118 160 202 244 286 



329 4 


4 

119 161 203 245 287 



330 5 


5 

120 162 204 246 288 



331 6 


6 

121 163 205 247 289 



332 7 


7 

122 164 206 248 290 

$ 


$ 

$ 


$ 

$ 

$================================== LOADING ==================================== 

$ 

*LOAD_SEGMENT 


1 1.000E+00 .000E+00 1 2 4 3 

1 1.000E+00 .000E+00 2 5 7 4 

1 1.000E+00 .000E+00 3 4 8 6 

1 1.000E+00 .000E+00 4 7 9 8 

$ 

$=============================== LOAD CURVES =================================== 

$ 

*DEFINE_CURVE 


1 0 .000E+00 .000E+00 .000E+00 .000E+00 

.00000000E+00 .53080000E+05 

.19999999E-03 .53080000E+05 

.20100000E-03 .00000000E+00 

.10000000E+01 .00000000E+00 

*END 

Page A.20


Results: 

OASYS D3PLOT: EXAMPLE OF SHELL BRICK INTERFACES 

Displacement 

0.10 

0.05 

-0.05 

-0.10 

-0.15 

-0.20 

0 

Undeformed Geometry 

Y 

Z 

X 

.000050 

0 5 10 15 20 25 30 35 40 

E-5 

Time 

Disp z - node 1 

EXAMPLE OF SHELL BRICK INTERFACES 



Version 7.0 

4-Feb-97 

Page A.21


LS-DYNA Manual Section: *CONTACT 

Example of: Shell Rebounds from Plate Using Five Contact Types 

Example Filenames: plate_type_3.key 

plate_type_4.key 




Description: 

A shell element drops and rebounds on an elastic plate. 

Model: 

The plate measures 40 × 40 × 1 mm 3 and contains 16 shell elements. The dropped shell element 

has a side length of 10 mm, a thickness of 2 mm and drop height of 10 mm. All shell elements are 

elastic with Belytschko-Tsay formulation. The dropped shell element has an initial velocity of 

100,000 mm/second vertically towards the plate. The calculations terminate at 0.0002 seconds. 

Input: 

All nodes have an initial velocity as specified above. (*INITIAL_VELOCITY). Contact types 3, 

5 and 10 use the dropped shell element as slave side and the four shell elements in the center of the 

plate as master side. 

Type 3 contact is a two way surface to surface algorithm. The segments on the slave side are 

checked for penetration of the master segment then the opposite search takes place. 

Type 4 is a single surface algorithm. The nodes of all segments are checked for penetration of all 

segments. 

Type 5 is a node to surface one way algorithm. The program checks that no slave node penetrates 

any master segment. 

Type 10 converts surface to surface definition into a node to surface definition. 

Type 13 is a more robust version of the single surface algorithm. It works especially well in the 

contact in airbag unfolding problems. 

Reference: 


Page A.22



CONTACT TYPE 3 

*KEYWORD 

*TITLE 

SLIDING INTERFACE TYPE 3 

$ 

$================================ CONTROL CARDS ================================ 

$ 




$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ] 

2.000E-04 0 .000E+00 .000E+00 .000E+00 





$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 0 0 0 0 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 .000E+00 0 0 1 0 0 




$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

0 0 0 0 .000E+00 




$ 1 ][ 2 ][ 3 ][ 4 ] 

1 0 1 1 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ][ 8 ] 

0 .000E+00 .000E+00 .000E+00 5.000E-01 0 .000E+00 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

0 0 0 0 .000E+00 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 5.000E-01 0 .000E+00 .000E+00 0 0 0 


4 .000E+00 

$ 


$ 

*DATABASE_MATSUM 

1.000E-06 

*DATABASE_NCFORC 

1.000E-06 

*DATABASE_RCFORC 

1.000E-06 


1.000E-05 0 1 



1.000E-06 0 


0 


0 

Page A.23



1.000E-05 0 


12 13 101 


0 0 0 1 0 0 0 0 

0 0 0 

$ 


$ 

*MAT_ELASTIC 

$ Material 1 : IMPACTED MATERIAL 

1 1.000E-08 1.000E+05 .3000 .000E+00 .000E+00 

$ 


$ 


$ Section 1 : IMPACTED MATERIAL 

1 0 .83330 2.0 3.0 .0 0 

1.000E+00 1.000E+00 1.000E+00 1.000E+00 .000E+00 

$------------------------------------------------------------------------------- 


$ Section 2 : IMPACTOR MATERIAL 

2 0 .83330 2.0 3.0 .0 0 

2.000E+00 2.000E+00 2.000E+00 2.000E+00 .000E+00 

$ 


$ 

*PART 

IMPACTED MATERIAL 

1 1 1 0 0 0 

$------------------------------------------------------------------------------- 

*PART 

IMPACTOR MATERIAL 

2 2 1 0 0 0 

$ 

$=================================== NODES ===================================== 

$ 

*NODE 


1 .00000000E+00 .00000000E+00 .00000000E+00 0 0 

... 104 .25000000E+02 .25000000E+02 .10000000E+02 0 0 

$ 

$================================== ELEMENTS =================================== 

$ 



1 1 1 2 7 6 

... 101 2 101 102 104 103 

$ 


$ 



1 1 1 1 1 0 0 0 

... 

25 1 1 1 1 0 0 0 


1 .0 .0 .0 1.0 .0 .0 

.0 1.0 .0 

$ 

$================================= CONSTRAINTS ================================= 

$ 

$ 


$ 

$ 


$ 


1 0 0 

.000E+00 .000E+00-1.000E+05 .000E+00 .000E+00 .000E+00 


1 

101 102 103 104 

$ 

$================================== LOADING ==================================== 

$ 

$ 

Page A.24



$ 

*CONTACT_SURFACE_TO_SURFACE_TITLE 

$ NUMBER NAME 

1 Contact # 1 


1 2 0 0 0 0 1 1 


.000E+00 .000E+00 .000E+00 .000E+00 .000E+00 0 .000E+00 .000E+00 


.000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 


0 .000E+00 0 .000E+00 .000E+00 0 0 0 


.000E+00 0 0 

*SET_SEGMENT 

1 .000E+00 .000E+00 .000E+00 .000E+00 

101 103 104 102 .000E+00 .000E+00 .000E+00 .000E+00 

*SET_SEGMENT 

2 .000E+00 .000E+00 .000E+00 .000E+00 

7 8 13 12 .000E+00 .000E+00 .000E+00 .000E+00 

8 9 14 13 .000E+00 .000E+00 .000E+00 .000E+00 

12 13 18 17 .000E+00 .000E+00 .000E+00 .000E+00 

13 14 19 18 .000E+00 .000E+00 .000E+00 .000E+00 

*END 


*CONTACT_SINGLE_SURFACE_TITLE 

$ NUMBER NAME 

1 Contact # 1 


1 0 0 0 0 0 1 1 


.000E+00 .000E+00 .000E+00 .000E+00 .000E+00 0 .000E+00 .000E+00 


.000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 


0 .000E+00 0 .000E+00 .000E+00 0 0 0 


.000E+00 0 0 

*SET_SEGMENT 

1 .000E+00 .000E+00 .000E+00 .000E+00 

101 103 104 102 .000E+00 .000E+00 .000E+00 .000E+00 

7 8 13 12 .000E+00 .000E+00 .000E+00 .000E+00 

8 9 14 13 .000E+00 .000E+00 .000E+00 .000E+00 

12 13 18 17 .000E+00 .000E+00 .000E+00 .000E+00 

13 14 19 18 .000E+00 .000E+00 .000E+00 .000E+00 



$ NUMBER NAME 

1 Contact # 1 


2 1 4 0 0 0 1 1 


.000E+00 .000E+00 .000E+00 .000E+00 .000E+00 0 .000E+00 .000E+00 


.000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 


0 .000E+00 0 .000E+00 .000E+00 0 0 0 


.000E+00 0 0 


2 

101 103 104 102 

*SET_SEGMENT 

1 .000E+00 .000E+00 .000E+00 .000E+00 

7 8 13 12 .000E+00 .000E+00 .000E+00 .000E+00 

8 9 14 13 .000E+00 .000E+00 .000E+00 .000E+00 

12 13 18 17 .000E+00 .000E+00 .000E+00 .000E+00 

13 14 19 18 .000E+00 .000E+00 .000E+00 .000E+00 

Page A.25



*CONTACT_ONE_WAY_SURFACE_TO_SURFACE_TITLE 

$ NUMBER NAME 

1 Contact # 1 


1 2 0 0 0 0 1 1 


.000E+00 .000E+00 .000E+00 .000E+00 .000E+00 0 .000E+00 .000E+00 


.000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 


0 .000E+00 0 .000E+00 .000E+00 0 0 0 


.000E+00 0 0 

*SET_SEGMENT 

1 .000E+00 .000E+00 .000E+00 .000E+00 

101 103 104 102 .000E+00 .000E+00 .000E+00 .000E+00 

*SET_SEGMENT 

2 .000E+00 .000E+00 .000E+00 .000E+00 

7 8 13 12 .000E+00 .000E+00 .000E+00 .000E+00 

8 9 14 13 .000E+00 .000E+00 .000E+00 .000E+00 

12 13 18 17 .000E+00 .000E+00 .000E+00 .000E+00 

13 14 19 18 .000E+00 .000E+00 .000E+00 .000E+00 


*CONTACT_AUTOMATIC_SINGLE_SURFACE_TITLE 

$ NUMBER NAME 

1 Contact # 1 


0 0 5 0 0 0 1 1 


.000E+00 .000E+00 .000E+00 .000E+00 .000E+00 0 .000E+00 .000E+00 


.000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 


0 .000E+00 0 .000E+00 .000E+00 0 0 0 


.000E+00 0 0 

Page A.26


Results: 

OASYS D3PLOT: SLIDING INTERFACE TYPE 3 

Force 

1 

0 

-1 

-2 

-3 

-4 

-5 

-6 

E4 

-7 

0 5 10 15 

E-5 

Time 

z force - surf 1 





Version 7.0 

4-Feb-97 

Z 

Y 

.000199 

X 

Page A.27


LS-DYNA Manual Section: *CONTACT_TIED_NODES_TO_SURFACE 

Example of: Discrete Nodes Tied to a Surface 

Example Filename: box_type_6.key 

Description: 

A shell element drops and rebounds onto an elastic plate with an attached hollow box. 

Model: 

The plate measures 40 × 40 × 1 mm 3 and contains 16 Belytschko-Tsay shell elements. The dropped 

shell element has a side length of 10 mm, a thickness of 2 mm and a drop height of 10 mm. The 

box measures 20 × 20 × 1 mm 3 and contains 12 Belytschko-Tsay shell elements. All shell element 

materials are elastic. The initial velocity of the shell elements is 100,000 mm/second. The 

calculation terminates at 0.002 seconds. 

Input: 

All nodes have initial velocity cards. (*INITIAL_VELOCITY) The box defines the nodes facing 

the plate as tied to the plate (*DEFINE_BOX, *CONTACT_TIED_NODES_TO_SURFACE). 

A type 3 surface to surface contact represents the interface between the dropped shells and the top 

surface of the box. A type 5 node to surface contact represents the middle node of the top surface 

of the box (‘slave’) and the elements of the plate (‘master’). The definition of the contact includes 

box and material input. The contact algorithms account for thickness of the shells 

(*CONTROL_CONTACT). 

Reference: 


Page A.28



*KEYWORD 

*TITLE 


$ 

$================================ CONTROL CARDS ================================ 

$ 




$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ] 

2.000E-04 0 .000E+00 .000E+00 .000E+00 





$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 0 0 0 0 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 .000E+00 0 0 1 0 0 




$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

0 0 0 0 .000E+00 




$ 1 ][ 2 ][ 3 ][ 4 ] 

0 0 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ][ 8 ] 

0 .000E+00 .000E+00 .000E+00 .000E+00 0 .000E+00 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

0 0 0 0 .000E+00 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 .000E+00 0 .000E+00 .000E+00 0 0 0 


4 .000E+00 

$ 


$ 

*DATABASE_NCFORC 

1.000E-04 


1.000E-05 0 1 


5.000E-07 0 


0 


0 


1.000E-05 0 


101 13 213 


0 0 0 0 0 0 0 0 

0 0 0 

$ 

Page A.29



$ 

*MAT_ELASTIC 

$ Material 1 : IMPACTED 

1 1.000E-08 1.000E+05 .3000 .000E+00 .000E+00 

$ 


$ 


$ Section 1 : IMPACTED 

1 0 .83330 2.0 .0 .0 0 

1.000E+00 1.000E+00 1.000E+00 1.000E+00 .000E+00 

$------------------------------------------------------------------------------- 


$ Section 2 : IMPACTOR 

2 0 .83330 2.0 .0 .0 0 

2.000E+00 2.000E+00 2.000E+00 2.000E+00 .000E+00 

$ 


$ 

*PART 

IMPACTED 1 1 1 0 0 0 

$------------------------------------------------------------------------------- 

*PART 

IMPACTOR 2 2 1 0 0 0 

$------------------------------------------------------------------------------- 

*PART 

IMPACTOR 3 1 1 0 0 0 

$ 

$=================================== NODES ===================================== 

$ 

*NODE 


1 .00000000E+00 .00000000E+00 .00000000E+00 0 0 

... 219 .20000000E+02 .34142101E+02 .10000000E+01 0 0 

$ 

$================================== ELEMENTS =================================== 

$ 



1 1 1 2 7 6 

... 212 3 215 216 219 218 

$ 


$ 



1 1 1 1 1 0 0 0 

... 

25 1 1 1 1 0 0 0 


1 .0 .0 .0 1.0 .0 .0 

.0 1.0 .0 

$ 

$================================= CONSTRAINTS ================================= 

$ 

$ 


$ 

$ 


$ 


1 0 0 

.000E+00 .000E+00-1.000E+05 .000E+00 .000E+00 .000E+00 


1 

101 102 103 104 

$ 

$================================== LOADING ==================================== 

$ 

$ 


$ 


$ NUMBER NAME 

Page A.30


1 Contact # 1 


1 2 2 2 1 0 1 1 


.000E+00 .000E+00 .000E+00 .000E+00 .000E+00 0 .000E+00 .000E+00 


.000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 


0 .000E+00 0 .000E+00 .000E+00 0 0 0 


.000E+00 0 0 

*DEFINE_BOX 

1 1.900E+01 2.100E+01 1.900E+01 2.100E+01 9.000E-01 1.100E+00 

*SET_PART 13 

*SET_PART 22 

$------------------------------------------------------------------------------- 


$ NUMBER NAME 

2 Contact # 2 


2 3 4 2 2 0 1 1 


.000E+00 .000E+00 .000E+00 .000E+00 .000E+00 0 .000E+00 .000E+00 


.000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 


0 .000E+00 0 .000E+00 .000E+00 0 0 0 


.000E+00 0 0 


2 

215 

*DEFINE_BOX 

2 1.900E+01 2.100E+01 1.900E+01 2.100E+01-1.000E-01 1.000E-01 

*SET_PART 31 

$------------------------------------------------------------------------------- 

*CONTACT_TIED_NODES_TO_SURFACE_TITLE 

$ NUMBER NAME 

3 Contact # 3 


3 4 4 2 0 0 1 1 


.000E+00 .000E+00 .000E+00 .000E+00 .000E+00 0 .000E+00 .000E+00 


.000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 


0 .000E+00 0 .000E+00 .000E+00 0 0 0 


.000E+00 0 0 


3 

201 202 203 204 206 207 208 209 

*SET_PART 41 

*END 

Page A.31


Results: 

OASYS D3PLOT: SLIDING INTERFACE TYPE 6 

Displacement 

2 

0 

-2 

-4 

-6 

-8 

-10 

Z 

Y 

.000200 

0 5 10 15 20 

E-5 

Time 







Version 7.0 

5-Feb-97 

X 

Page A.32


LS-DYNA Manual Section: *CONTACT_ERODING_SURFACE_TO_SURFACE 

Example of: Projectile penetrates Plate 

Example Filename: projectile_plate.key 

Description: 

A projectile strikes a plate at a critical angle. 

Model: 

The hemispherical projectile has a length of 7.67 cm and a diameter of 0.767 cm. The plate 

measures 23.01 cm × 23 cm × 0.64 cm. The projectile and the plate are elastic perfectly plastic with 

failure strain. The initial velocity of the projectile is 0.129 cm/µsec at an angle of 75 degrees. The 

calculation terminates at 110.0 µsec. 

Input: 

All nodes have initial velocity cards (*INITIAL_VELOCITY) 

A type 14 eroding surface to surface with the bucket sorting algorithm contact represents the 

interface between the projectile material and the plate material 

(*CONTACT_ERODING_SURFACE_TO_SURFACE). 

Results: 

The projectile fractures into a tip and trailing portion. The trailing portion punches a hole through 

the plate while the tip reflects off the plate. 

Page A.33



*KEYWORD 

*TITLE 

PROJECTILE PENETRATING PLATE 

$ 

$================================ CONTROL CARDS ================================ 

$ 




$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ] 

1.100E+02 0 .000E+00 .000E+00 .000E+00 





$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 0 0 0 0 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

1.000E+00 .000E+00 0 0 1 0 0 




$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

0 0 0 0 .000E+00 




$ 1 ][ 2 ][ 3 ][ 4 ] 

0 0 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ][ 8 ] 

0 .000E+00 .000E+00 .000E+00 .000E+00 0 .000E+00 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

0 0 0 0 .000E+00 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 .000E+00 0 .000E+00 .000E+00 0 0 0 

$ 


$ 


1.000E+01 0 1 



1.000E+01 0 


0 


0 


1.000E+01 0 


0 0 0 0 0 0 0 0 

0 0 0 

$ 


$ 

*MAT_PLASTIC_KINEMATIC 

$ Material 1 : STEEL 

Page A.34


1 1.862E+01 1.170E+00 .2200 1.790E-02 .000E+00 1.000E+00 

.000E+00 .000E+00 8.000E-01 

$------------------------------------------------------------------------------- 


$ Material 2 : PENTRATOR 

2 7.896E+00 2.100E+00 .2840 1.000E-02 .000E+00 1.000E+00 

.000E+00 .000E+00 8.000E-01 

$ 


$ 


$ Section 1 : STEEL 

1 0 

$ 


$ 

*PART 

STEEL 

1 1 1 0 0 0 

$------------------------------------------------------------------------------- 

*PART 

PENTRATOR 2 1 2 0 0 0 

$ 

$=================================== NODES ===================================== 

$ 

*NODE 


1 .92417507E+01 -.15340000E-04 .51379278E-01 0 0 

... 7668 .23000000E+02 .48000002E+01 .00000000E+00 0 0 

$ 

$================================== ELEMENTS =================================== 

$ 



1 1 1 2 5 4 10 11 14 13 

... 5664 2 7619 7620 7628 7627 7659 7660 7668 7667 

$ 


$ 



1 1 0 1 0 1 0 1 

... 

7668 1 1 1 1 1 1 1 


1 .0 .0 .0 1.0 .0 .0 

.0 1.0 .0 

$ 

$================================= CONSTRAINTS ================================= 

$ 

$ 


$ 

$ 


$ 


1 0 0 

1.246E-01 .000E+00-3.339E-02 .000E+00 .000E+00 .000E+00 


1 

1 2 3 4 5 6 7 8 

... 

2585 2586 

$ 

$================================== LOADING ==================================== 

$ 

$ 


$ 

*CONTACT_ERODING_SURFACE_TO_SURFACE_TITLE 

$ NUMBER NAME 

1 Contact # 1 


1 2 2 2 0 0 0 0 


.000E+00 .000E+00 .000E+00 .000E+00 .000E+00 0 .000E+00 .000E+00 


Page A.35


.000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 

$ SYMMETRY EROSION ADJACENT 

1 1 0 


0 .000E+00 0 .000E+00 .000E+00 0 0 0 


.000E+00 0 0 

*SET_PART 11 

*SET_PART 22 

*END 

Page A.36


Results: 

OASYS D3PLOT: PROJECTILE PENETRATING PLATE 

OASYS D3PLOT: PROJECTILE PENETRATING PLATE 

Y 

Z 

X 

.000000000 

Y 

Z 

X 

109.971863 

Page A.37


LS-DYNA Manual Section: *CONTACT_SINGLE_EDGE 

Example of: Corrugated Sheet Contacts Edges 

Example File Name: edge_to_edge.key 

Description: 

A corrugated plate strikes a flat plate from opposite directions. 

Input: 

The model consists of 135 elastic plastic Belytschko-Tsay shell elements. The interaction of the 

two structures is modelled using an edge to edge contact (*CONTACT_SINGLE_EDGE). The 

nodes on the upper corrugated plate have an initial velocity of 10 meters/second. 

Results: 

A contour plot of z-stress illustrates that the plates are in contact. 

Reference: 

Stillman, D. W. 

Page A.38



*KEYWORD 

*TITLE 

EDGE TO EDGE CONTACT 

$ 

$================================ CONTROL CARDS ================================ 

$ 




$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ] 

5.000E-01 0 .000E+00 .000E+00 .000E+00 





$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 0 0 0 0 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 .000E+00 0 0 1 0 0 




$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

0 0 0 0 .000E+00 




$ 1 ][ 2 ][ 3 ][ 4 ] 

0 0 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ][ 8 ] 

0 .000E+00 .000E+00 .000E+00 .000E+00 0 .000E+00 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

0 0 0 0 .000E+00 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 .000E+00 0 .000E+00 .000E+00 0 0 0 


4 .000E+00 

$ 


$ 


5.000E-01 

*DATABASE_RBDOUT 

5.000E-01 


1.000E-03 0 1 



9.990E+02 0 


0 


0 


1.000E-03 0 


0 0 0 0 0 0 0 0 

Page A.39


0 0 0 

$ 


$ 


$ Material 1 : SHELL 1 -STEEL 

1 7.850E+03 2.000E+11 .3000 2.000E+09 .000E+00 .000E+00 

.000E+00 .000E+00 .000E+00 

$ 


$ 


$ Section 1 : SHELL 1 -STEEL 

1 0 .00000 .0 .0 .0 0 

2.000E-03 2.000E-03 2.000E-03 2.000E-03 .000E+00 

$ 


$ 

*PART 

SHELL 1 -STEEL 

1 1 1 0 0 0 

$------------------------------------------------------------------------------- 

*PART 


2 1 1 0 0 0 

$------------------------------------------------------------------------------- 

*PART 


3 1 1 0 0 0 

$ 

$=================================== NODES ===================================== 

$ 

*NODE 


1 .00000000E+00 -.10000000E+00 .15000000E+01 0 0 

... 192 .20000000E+02 .81000004E+01 -.15000000E+01 0 0 

$ 

$================================== ELEMENTS =================================== 

$ 



1 1 1 4 5 2 

... 135 3 189 191 192 190 

$ 


$ 

$ 

$================================= CONSTRAINTS ================================= 

$ 

$ 


$ 

$ 


$ 


1 0 0 

.000E+00 1.000E+01 .000E+00 .000E+00 .000E+00 .000E+00 


1 

1 2 3 4 5 6 7 8 

... 

65 66 67 68 

$ 

$================================== LOADING ==================================== 

$ 

$ 


$ 

*CONTACT_SINGLE_EDGE_TITLE 

$ NUMBER NAME 

1 Contact # 1 


1 0 0 0 0 0 0 0 


.000E+00 .000E+00 .000E+00 .000E+00 .000E+00 0 .000E+00 .000E+00 


.000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 


Page A.40


0 .000E+00 0 .000E+00 .000E+00 0 0 0 


.000E+00 0 0 

*SET_SEGMENT 

1 .000E+00 .000E+00 .000E+00 .000E+00 

1 2 0 0 .000E+00 .000E+00 .000E+00 .000E+00 

... 

185 186 0 0 .000E+00 .000E+00 .000E+00 .000E+00 

*END 

Page A.41


Results: 

OASYS D3PLOT: EDGE TO EDGE CONTACT 

OASYS D3PLOT: EDGE TO EDGE CONTACT 

Y 

Z 

X 

.000000000 

GLOBAL Z_DIRECT_STRESS 

(Mid surface) 

-55.25 

-33.81 

-12.37 

9.07 

30.52 

51.96 

73.40 

x 1.0E+06 

Y 

Z 

.029910 

X 

Page A.42


LS-DYNA Manual Section: *CONTACT_ENTITY 

Example of: Rigid Sphere impacts Plate 

Example Filename: sphere_geometric.key 

Description: 

A rigid sphere drops onto an elastic plate. The sphere contains shell elements automatically 

generated with a Geometric Contact Entity spherical surface. 

Model: 

The plate of elastic material measures 40 × 40 × 2 mm 3 and contains 64 Belytschko-Tsay shell 

elements. The sphere has a radius of 6.0 mm and the distance from the center of the cube to the 

plate is 8.5 mm. The inertia properties of the sphere are defined by the properties of the rigid brick 

element. A geometric contact entity defines the spherical contact surface. 

The sphere moves toward the plate with a uniform motion. The termination time is 0.0005 seconds. 

Input: 

The Geometric Contact Entity defines the outer master surface on the rigid sphere 

(*CONTACT_ENTITY). The nodes on the plate are slave nodes (*SET_NODE_LIST) , and are 

in the Geometric Entity. 

A load curve definition defines the movement of the sphere (*PRESCRIBED_MOTION_RIGID, 

*DEFINE_CURVE). The displacement condition for rigid bodies is input by material numbers, not 

by listing the nodes included in the definition. 

Reference: 


Page A.43



*KEYWORD 

*TITLE 

GEOMETRIC CONTACT ENTITY 

$ 

$================================ CONTROL CARDS ================================ 

$ 

*CONTROL_STRUCTURED 




$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ] 

5.000E-04 0 .000E+00 .000E+00 .000E+00 





$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 0 0 0 0 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 .000E+00 0 0 1 0 0 




$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

0 0 0 0 .000E+00 




$ 1 ][ 2 ][ 3 ][ 4 ] 

0 0 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ][ 8 ] 

0 .000E+00 .000E+00 .000E+00 1.000E-01 0 .000E+00 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

0 0 0 0 .000E+00 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 1.000E-01 0 .000E+00 .000E+00 0 0 0 


4 .000E+00 

$ 


$ 

*DATABASE_RBDOUT 

5.000E-06 

*DATABASE_GCEOUT 

5.000E-06 


2.000E-05 0 1 



.000E+00 0 


0 


0 


2.000E-05 0 


Page A.44


0 0 0 0 0 0 0 0 

0 0 0 

$ 


$ 

*MAT_ELASTIC 

$ Material 1 : ELASTIC 

1 2.000E-08 1.000E+05 .3000 .000E+00 .000E+00 

$------------------------------------------------------------------------------- 

*MAT_RIGID 

$ Material 2 : RIGID MATERIAL 

2 2.000E-08 1.000E+05 .3000 .0 4.0 .0 

.0 .0 .0 

.000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 

$ 


$ 


$ Section 1 : ELASTIC 

1 0 .83330 2.0 3.0 .0 0 

2.000E+00 2.000E+00 2.000E+00 2.000E+00 .000E+00 

$------------------------------------------------------------------------------- 


$ Section 2 : RIGID MATERIAL 

2 0 

$ 


$ 

*PART 

ELASTIC 

1 1 1 0 0 0 

$------------------------------------------------------------------------------- 

*PART 

RIGID MATERIAL 

2 2 2 0 0 0 

$ 

$=================================== NODES ===================================== 

$ 

*NODE 


1 .00000000E+00 .00000000E+00 .00000000E+00 0 0 

... 

81 .40000000E+02 .40000000E+02 .00000000E+00 0 0 

$ 

$================================== ELEMENTS =================================== 

$ 



1 1 1 2 11 10 

... 

64 1 71 72 81 80 

$ 


$ 



1 1 0 0 1 0 0 0 

... 

81 1 0 0 1 0 0 0 


1 .0 .0 .0 1.0 .0 .0 

.0 1.0 .0 

*BOUNDARY_PRESCRIBED_MOTION_RIGID 

$ PART ID DOF TYPE CURVE ID FACTOR VECT ID 

2 3 2 1 1.000E+00 0 .000E+00 

$ 

$================================= CONSTRAINTS ================================= 

$ 

$ 


$ 

$ 


$ 


0 0 1 

.000E+00 .000E+00-3.000E+04 .000E+00 .000E+00 .000E+00 

*DEFINE_BOX 

1-1.000E+02 1.000E+02-1.000E+02 1.000E+02 3.000E+00 1.500E+01 

$ 


Page A.45


$ 

*CONTACT_ENTITY 

$ i i i i f f f i 

$ PART ID TYPE SET ID SET TYPE FACTOR DAMPING COULOMB ORDER 

2 2 1 0 1.0 

$ BIRTH DEATH FLAG MESH 

0.0 0.0 0 1 

$ X-COORD Y-COORD Z-COORD LOCAL AX LOCAL AY LOCAL AZ 

0.00 0.00 .00 1.00 0.00 0.00 

$ LOCAL BX LOCAL BY LOCAL BZ 

0.00 1.00 0.00 

$ INOUT G1 G2 G3 G4 G5 G6 G7 

0 20.00 20.00 9.00 6.00 


1 

1 2 3 4 5 6 7 8 

... 

81 

$ 

$================================== LOADING ==================================== 

$ 

$ 

$=============================== LOAD CURVES =================================== 

$ 

*DEFINE_CURVE 


1 0 .000E+00 .000E+00 .000E+00 .000E+00 

.00000000E+00 .00000000E+00 

.49999999E-02 -.15000000E+03 

*END 

Page A.46


Results: 

OASYS D3PLOT: GEOMETRIC CONTACT ENTITY 

Displacment 

0 

-2 

-4 

-6 

-8 

-10 

-12 

-14 

-16 

Z 

Y 

.000360 

0 1 2 3 4 5 

E-4 

Time 

Disp z - Mat #2 

GEOMETRIC CONTACT ENTITY 



Version 7.0 

4-Feb-97 

X 

Page A.47


LS-DYNA Manual Section: *CONTROL_CONTACT 

Example of: Hemispherical Punch 

Example Filenames: hemi_draw.key 

Description: 

This problem includes three tools a punch, a pressure pad, a die and a workpiece. A workpiece is 

deep drawn by the hemispherical punch while the pressure pad and die prevents wrinkling. The 

load on the pressure pad is ramped, then the punch displaces in the y direction. 

Model: 

The workpiece measures 80 mm in radius and 1 mm in thickness. The punch radius is 50.0 mm and 

the die torus radius is 6.35 mm. The workpiece contains 528 Belytschko Tsay shell elements with 

5 integration points through the thickness. The tools are rigid members. 

Input: 

The number of integration points is 5 for the workpiece. (*SECTION_SHELL) This model contains 

two options to consider shell thickness. The first option is the contact surfaces are projected to the 

true surface of shell (*CONTROL_CONTACT). The second option is membrane straining results 

in thickness changes (*CONTROL_CONTACT). The motion of the punch follows a sine function 

represented by load curve number 2 (Section 22). 

Results: 

The plots show an exploded view of the parts, thickness at an intermediate step, and resultant forces 

at the contact interfaces. 

Reference: 

Honecker, A. and Mattiason, K. 

Page A.48



*KEYWORD 

*TITLE 

HEMISPHERICAL DEEP DRAW 

$ 

$================================ CONTROL CARDS ================================ 

$ 




$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ] 

6.000E+00 0 .000E+00 .000E+00 .000E+00 





$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

2.000E+01 2 -1 1 2 2 1 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 1.000E+00 0 1 1 0 0 




$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

0 0 0 0 .000E+00 




$ 1 ][ 2 ][ 3 ][ 4 ] 

2 0 2 1 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ][ 8 ] 

0 .000E+00 .000E+00 .000E+00 .000E+00 0 .000E+00 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

0 0 0 0 .000E+00 2 1000 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 .000E+00 0 .000E+00 .000E+00 0 0 0 

$ 


$ 


5.000E-02 


2.000E-01 0 1 



5.000E-02 0 


0 


0 


2.000E-01 0 


1333 


0 0 0 1 0 0 0 0 

0 0 0 

$ 

Page A.49



$ 

*MAT_POWER_LAW_PLASTICITY 

$ Material 1 : POWER LAW PLASTICITY - WORKPIECE 

1 7.830E-06 6.900E+01 .3000 5.980E-01 2.160E-01 .000E+00 .000E+00 

$------------------------------------------------------------------------------- 

*MAT_RIGID 

$ Material 2 : RIGID - PUNCH 

2 7.830E-06 6.900E+01 .3000 .0 .0 .0 

.0 .0 .0 

.000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 

$ 


$ 


$ Section 1 : POWER LAW PLASTICITY - WORKPIECE 

1 2 .00000 5.0 .0 .0 0 

1.000E+00 1.000E+00 1.000E+00 1.000E+00 .000E+00 

$ 


$ 

*PART 

POWER LAW PLASTICITY - WORKPIECE 

1 1 1 0 0 0 

$------------------------------------------------------------------------------- 

*PART 

RIGID - PUNCH 

2 1 2 0 0 0 

$------------------------------------------------------------------------------- 

*PART 

RIGID - PUNCH 

3 1 2 0 0 0 

$------------------------------------------------------------------------------- 

*PART 

RIGID - PUNCH 

4 1 2 0 0 0 

$ 

$=================================== NODES ===================================== 

$ 

*NODE 


1 .00000000E+00 .00000000E+00 .00000000E+00 0 0 

... 1599 .00000000E+00 -.50005352E+00 -.80800003E+02 0 0 

$ 

$================================== ELEMENTS =================================== 

$ 



1 1 1 8 9 2 

... 1452 4 1591 1598 1599 1592 

$ 


$ 



1 1 1 0 1 1 1 1 

... 

1599 1 1 1 1 1 1 1 


1 .0 .0 .0 1.0 .0 .0 

.0 1.0 .0 



2 2 0 2-1.000E+00 0 .000E+00 

$ 

$================================= CONSTRAINTS ================================= 

$ 

$ 


$ 

*RIGIDWALL_PLANAR 

1 0 0 

$ X-TAIL Y-TAIL Z-TAIL X-HEAD Y-HEAD Z-HEAD FRICTION 

.000E+00 .000E+00 .000E+00 .000E+00 1.000E+00 .000E+00 .000E+00 


1 

900 901 902 903 904 905 906 907 

... 

1068 1069 1070 1071 1072 1073 1074 

Page A.50


$ 


$ 

$ 

$================================== LOADING ==================================== 

$ 

*LOAD_SEGMENT 


1 1.000E+00 .000E+00 907 900 901 908 

... 

1 1.000E+00 .000E+00 1073 1066 1067 1074 

$ 


$ 


$ NUMBER NAME 

1 Contact # 1 


1 2 2 2 0 0 0 0 


1.500E-01 1.500E-01 .000E+00 .000E+00 .000E+00 0 .000E+00 .000E+00 


.000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 


0 .000E+00 0 .000E+00 .000E+00 0 0 0 


.000E+00 0 0 

*SET_PART 11 

*SET_PART 22 

$------------------------------------------------------------------------------- 


$ NUMBER NAME 

2 Contact # 2 


3 4 2 2 0 0 0 0 


1.500E-01 1.500E-01 .000E+00 .000E+00 .000E+00 0 .000E+00 .000E+00 


.000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 


0 .000E+00 0 .000E+00 .000E+00 0 0 0 


.000E+00 0 0 

*SET_PART 31 

*SET_PART 43 

$------------------------------------------------------------------------------- 


$ NUMBER NAME 

3 Contact # 3 


5 6 2 2 0 0 0 0 


1.500E-01 1.500E-01 .000E+00 .000E+00 .000E+00 0 .000E+00 .000E+00 


.000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 


0 .000E+00 0 .000E+00 .000E+00 0 0 0 


.000E+00 0 0 

*SET_PART 51 

*SET_PART 64 

$ 

$=============================== LOAD CURVES =================================== 

$ 

*DEFINE_CURVE 


1 0 .000E+00 .000E+00 .000E+00 .000E+00 

.00000000E+00 .00000000E+00 

.10000000E+01 .10000000E-02 

Page A.51


.60000000E+01 .10000000E-02 

*DEFINE_CURVE 


2 0 .000E+00 .000E+00 .000E+00 .000E+00 

.00000000E+00 .00000000E+00 

... 

.60000000E+01 .00000000E+00 

*DEFINE_CURVE 


3 0 .000E+00 .000E+00 .000E+00 .000E+00 

.00000000E+00 .00000000E+00 

.60000000E+01 .00000000E+00 

*END 

Page A.52


Results: 

OASYS D3PLOT: HEMISPHERICAL DEEP DRAW 

OASYS D3PLOT: HEMISPHERICAL DEEP DRAW 

THICKNESS 

.875 

.908 

.941 

.975 

1.008 

1.041 

1.074 

Y 

X 

Z 

4.199544 

Y 

X 

Z 

4.199544 

Page A.53


Force 

20 

18 

16 

14 

12 

10 

8 

6 

4 

2 

0 

0 1 2 3 

Time 

4 5 6 

mag force - surf 1 



HEMISPHERICAL DEEP DRAW 



Version 7.0 

5-Feb-97 

Page A.54


LS-DYNA Manual Section: *CONTROL_DAMPING 

Example of: Cantilever Beam 

Example Filenames: beam_free.key 

beam_damping.key 

Description: 

A cantilever beam is subjected to a load at the free end. The beam then vibrates relative to the 

equilibrium position without damping in case 1 and with damping in case 2. 

Model: 

The beam measures 1000 × 100 × 10 mm 3 and is modeled by 10 Belytschko-Tsay shell elements. 

A force of 10 N is applied in the z-direction at the free end. The calculation ends at 0.5 seconds. 

Input for the undamped system: 

The load at the free end is applied as two point forces. The size of these forces is controlled by load 

curve definition number 1 (*DEFINE_CURVE, *LOAD_NODE_SET). 

Input for the damped system: 

The same input as in the undamped case except for a global damping constant 

(*DAMPING_GLOBAL, *CONTROL_DAMPING). 

Reference: 


Page A.55


List of first LS-DYNA input deck: 

*KEYWORD 

*TITLE 

CANTILEVER BEAM WITHOUT DAMPING 

$ 

$================================ CONTROL CARDS ================================ 

$ 




$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ] 

5.001E-01 0 .000E+00 .000E+00 .000E+00 





$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 0 0 0 0 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

1.000E-01 .000E+00 0 0 1 0 0 




$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

0 0 0 0 .000E+00 




$ 1 ][ 2 ][ 3 ][ 4 ] 

0 0 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ][ 8 ] 

100 1.000E-03 9.950E-01 .000E+00 9.000E-01 0 .000E+00 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

0 0 0 0 .000E+00 2 1000 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 .000E+00 0 .000E+00 .000E+00 0 0 0 


4 .000E+00 

$ 


$ 

*DATABASE_SECFORC 

5.000E-03 

*DATABASE_NODOUT 

1.000E-03 

*DATABASE_ELOUT 

5.000E-01 


5.000E-02 0 1 



5.000E-03 0 


0 


0 


5.000E-02 0 

Page A.56



21 


1 


0 0 0 1 0 0 0 0 

0 0 0 

$ CROSS SECTION 1 

*DATABASE_CROSS_SECTION_SET 

1 0 0 1 0 0 


1 

1 2 

*SET_SHELL_LIST 

1 

1 

$ 


$ 

*MAT_ELASTIC 

$ Material 1 : BEAM - ELASTIC MATERIAL 

1 1.000E-08 2.100E+05 .3000 .000E+00 .000E+00 

$ 


$ 


$ Section 1 : BEAM - ELASTIC MATERIAL 

1 2 1.00000 2.0 1.0 .0 0 

1.000E+01 1.000E+01 1.000E+01 1.000E+01 .000E+00 

$ 


$ 

*PART 

BEAM - ELASTIC MATERIAL 

1 1 1 0 0 0 

$ 

$=================================== NODES ===================================== 

$ 

*NODE 


1 .00000000E+00 .00000000E+00 .00000000E+00 0 0 

... 

22 .10000000E+04 .10000000E+03 .00000000E+00 0 0 

$ 

$================================== ELEMENTS =================================== 

$ 



1 1 1 3 4 2 

... 

10 1 19 21 22 20 

$ 


$ 



1 1 1 1 1 1 1 1 

2 1 1 1 1 1 1 1 


1 .0 .0 .0 1.0 .0 .0 

.0 1.0 .0 

$ 

$================================= CONSTRAINTS ================================= 

$ 

$ 


$ 

$ 


$ 

$ 

$================================== LOADING ==================================== 

$ 



21 3 1 5.000E-01 0 0 0 0 

22 3 1 5.000E-01 0 0 0 0 

$ 

$=============================== LOAD CURVES =================================== 

$ 

*DEFINE_CURVE 

Page A.57



1 0 .000E+00 .000E+00 .000E+00 .000E+00 

.00000000E+00 .10000000E+03 

.10000000E+02 .10000000E+03 

*END 

List of second LS-DYNA input deck 

*KEYWORD 

*TITLE 

CANTILEVER BEAM WITH DAMPING 

$ 

$================================ CONTROL CARDS ================================ 

$ 




$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ] 

5.001E-01 0 .000E+00 .000E+00 .000E+00 





$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 0 0 0 0 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

1.000E-01 .000E+00 0 0 1 0 0 




$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

0 0 0 0 .000E+00 




$ 1 ][ 2 ][ 3 ][ 4 ] 

0 0 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ][ 8 ] 

100 1.000E-03 9.950E-01 .000E+00 9.000E-01 0 .000E+00 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

0 0 0 0 .000E+00 2 1000 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 .000E+00 0 .000E+00 .000E+00 0 0 0 


4 .000E+00 

$ 


$ 


5.000E-03 


1.000E-03 


5.000E-01 


5.000E-02 0 1 

*DATBASE_BINARY_XTFILE 

Page A.58



5.000E-03 0 


0 


0 


5.000E-02 0 


21 


1 


0 0 0 1 0 0 0 0 

0 0 0 



1 0 0 1 0 0 


1 

1 2 


1 

1 

$ 


$ 

*MAT_ELASTIC 

$ Material 1 : BEAM - ELASTIC MATERIAL 

1 1.000E-08 2.100E+05 .3000 .000E+00 .000E+00 

$ 


$ 


$ Section 1 : BEAM - ELASTIC MATERIAL 

1 2 1.00000 2.0 1.0 .0 0 

1.000E+01 1.000E+01 1.000E+01 1.000E+01 .000E+00 

$ 


$ 

*PART 

BEAM - ELASTIC MATERIAL 

1 1 1 0 0 0 

$ 

$=================================== NODES ===================================== 

$ 

*NODE 


1 .00000000E+00 .00000000E+00 .00000000E+00 0 0 

... 

22 .10000000E+04 .10000000E+03 .00000000E+00 0 0 

$ 

$================================== ELEMENTS =================================== 

$ 



1 1 1 3 4 2 

... 

10 1 19 21 22 20 

*DAMPING_GLOBAL 

0 5.000E+01 

$ 


$ 



1 1 1 1 1 1 1 1 

2 1 1 1 1 1 1 1 


1 .0 .0 .0 1.0 .0 .0 

.0 1.0 .0 

$ 

$================================= CONSTRAINTS ================================= 

$ 

$ 


$ 

$ 


$ 

$ 

Page A.59


$================================== LOADING ==================================== 

$ 



21 3 1 5.000E-01 0 0 0 0 

22 3 1 5.000E-01 0 0 0 0 

$ 

$=============================== LOAD CURVES =================================== 

$ 

*DEFINE_CURVE 


1 0 .000E+00 .000E+00 .000E+00 .000E+00 

.00000000E+00 .10000000E+03 

.10000000E+02 .10000000E+03 

*END 

Page A.60


Results: 

Displacement 

Displacement 

40 

35 

30 

25 

20 

15 

10 

5 

CANTILEVER BEAM WITHOUT DAMPING 

0 

0 0.1 0.2 0.3 0.4 0.5 

Time 


40 

35 

30 

25 

20 

15 

10 

5 



Version 7.0 

5-Feb-97 

0 

0 0.1 0.2 0.3 0.4 0.5 

Time 


CANTILEVER BEAM WITH DAMPING 



Version 7.0 

5-Feb-97 

Page A.61


LS-DYNA Manual Section: *CONTROL_ENERGY 

Example of: Bar Impact 

Example Filenames: bar_impact.key 

Description: 

A copper bar strikes a wall. 

Model: 

A 1/4 symmetry bar measures 0.32 cm in radius and 3.24 cm in length and contains 972 hexahedron 

element. The bar starts at 0.0227 cm/sec and stops at 0 cm/µsec. The calculation illustrates the 

energy balance where E = KE + IE + HGE. 

Input: 

The hourglass energy is computed at a negligible cost. (*CONTROL_ENERGY) The initial 

velocity for every node is set to -0.0227 except the nodes at z = 0. 

Results: 

The displacements and plastic strains are provided in the figures. The balance of energy is shown 

in the last figure. 

Page A.62



*KEYWORD 

*TITLE 

BAR IMPACT 

$ 

$================================ CONTROL CARDS ================================ 

$ 




$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ] 

8.210E+01 0 .000E+00 .000E+00 .000E+00 





$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 0 0 0 0 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 .000E+00 0 0 1 0 0 




$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

0 0 0 0 .000E+00 




$ 1 ][ 2 ][ 3 ][ 4 ] 

2 0 1 1 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ][ 8 ] 

0 .000E+00 .000E+00 .000E+00 .000E+00 0 .000E+00 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

0 0 0 0 .000E+00 2 1000 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 .000E+00 0 .000E+00 .000E+00 0 0 0 


4 .000E+00 

$ 


$ 


1.000E+00 


2.500E+00 0 1 



1.000E+00 0 


0 


0 


2.500E+00 0 


1333 


0 0 0 0 0 0 0 0 

Page A.63


0 0 0 

$ 


$ 


$ Material 1 : ELASTIC PLASTIC MATERIAL 

1 8.930E+00 1.170E+00 .3500 4.000E-03 1.000E-03 1.000E+00 

.000E+00 .000E+00 .000E+00 

$ 


$ 


$ Section 1 : ELASTIC PLASTIC MATERIAL 

1 0 

$ 


$ 

*PART 

ELASTIC PLASTIC MATERIAL 

1 1 1 0 0 0 

$ 

$=================================== NODES ===================================== 

$ 

*NODE 


1 .00000000E+00 .00000000E+00 .00000000E+00 0 0 

... 1369 .00000000E+00 .31999999E+00 .32400000E+01 0 0 

$ 

$================================== ELEMENTS =================================== 

$ 



1 1 8 1 2 9 45 38 39 46 

... 972 1 1331 1328 1329 1332 1368 1365 1366 1369 

$ 


$ 



1 1 1 1 1 1 1 1 

... 

1369 1 1 0 0 1 1 1 


1 .0 .0 .0 1.0 .0 .0 

.0 1.0 .0 

$ 

$================================= CONSTRAINTS ================================= 

$ 

$ 


$ 

$ 


$ 


0 0 1 

.000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 

*DEFINE_BOX 

1-1.000E+06 1.000E+06-1.000E+06 1.000E+06-1.000E+06 5.000E-03 


0 0 2 

.000E+00 .000E+00-2.270E-02 .000E+00 .000E+00 .000E+00 

*DEFINE_BOX 

2-1.000E+06 1.000E+06-1.000E+06 1.000E+06 5.000E-03 1.000E+06 

$ 

$================================== LOADING ==================================== 

$ 

*END 

Page A.64


Results: 

OASYS D3PLOT: BAR IMPACT 


Z 

Y 

X 

.000000000 

Z_DISPLACEMENT 

-1.126 

-1.013 

-.901 

-.788 

-.675 

-.563 

-.450 

-.338 

-.225 

-.113 

.000 

Z 

Y 

79.987305 

X 

Page A.65



Energy 

6 

5 

4 

3 

2 

PLASTIC_STRAIN 

.000 

.178 

.356 

.535 

.713 

.891 

1.069 

1.247 

1.426 

1.604 

1.782 

Z 

Y 

79.987305 

1 

E-4 

0 

0 10 20 30 40 

Time 

50 60 70 80 

K.E. - total 

I.E. - total 

HG.E - total 

Total 

BAR IMPACT 



Version 7.0 

5-Feb-97 

X 

Page A.66


LS-DYNA Manual Section: *CONTROL_SHELL 

Example of: Hemispherical Load 

Example Filenames: hemi_load.key 

Description: 

A spherical shell is subjected to two outward point loads on the x-axis and two inward point loads 

on the y-axis. 

Model: 

The 1/8 symmetry model of a sphere measures 10 inches in radius with a thickness of 0.04 inches. 

The model contains 48 shell elements. A force of one pound is applied in the positive x-direction 

to the node on the x-axis. A force of one pound is applied in the negative y-direction to the node 

on the y-axis. The calculation terminates at 0.018 seconds. 

Input: 

The element formulation used is the Hughes-Liu shell. If the Belytschko Tsay shell was used 

the Belytschko-Wang-Chiang warpage stiffness option (*CONTROL_SHELL) would also have to 

be use. The concentrated loads are applied to two nodes (*DEFINE_CURVE, 

*LOAD_NODE_POINT). 

Results: 

The oscillation of the node on the z-axis shows a regular oscillatory behavior. 

Reference: 

Belytschko, T., Wang and Chiang. 

Page A.67



*KEYWORD 

*TITLE 

HEMISPHERICAL SHELL 

$ 

$================================ CONTROL CARDS ================================ 

$ 




$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ] 

6.000E-02 0 .000E+00 .000E+00 .000E+00 





$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

2.000E+01 2 -2 0 1 2 1 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 .000E+00 0 0 1 0 0 




$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

0 0 0 0 .000E+00 




$ 1 ][ 2 ][ 3 ][ 4 ] 

2 0 1 1 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ][ 8 ] 

0 .000E+00 .000E+00 .000E+00 .000E+00 0 .000E+00 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

0 0 0 0 .000E+00 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 .000E+00 0 .000E+00 .000E+00 0 0 0 


4 .000E+00 

$ 


$ 


6.000E-04 0 1 



1.000E-05 0 


0 


0 


6.000E-04 0 


1 


0 0 0 0 0 0 0 0 

0 0 0 

$ 

Page A.68



$ 


$ Material 1 : SHELL - PLASTIC 

1 1.000E-03 6.825E+07 .3000 6.000E+05 .000E+00 .000E+00 

.000E+00 .000E+00 .000E+00 

$ 


$ 


$ Section 1 : SHELL - PLASTIC 

1 0 .00000 5.0 .0 .0 0 

4.000E-02 4.000E-02 4.000E-02 4.000E-02 .000E+00 

$ 


$ 

*PART 

SHELL - PLASTIC 

1 1 1 0 0 0 

$ 

$=================================== NODES ===================================== 

$ 

*NODE 


1 .00000000E+00 .00000000E+00 .10000000E+02 0 0 

... 

61 .71679339E+01 .49305539E+01 .49305539E+01 0 0 

$ 

$================================== ELEMENTS =================================== 

$ 



1 1 1 6 7 2 

... 

48 1 61 20 25 45 

$ 


$ 



1 1 1 0 0 0 1 1 

... 

49 1 0 0 1 1 1 0 


1 .0 .0 .0 1.0 .0 .0 

.0 1.0 .0 

$ 

$================================= CONSTRAINTS ================================= 

$ 

$ 


$ 

$ 


$ 

$ 

$================================== LOADING ==================================== 

$ 



46 1 1-1.000E+00 0 0 0 0 

1 3 1 1.000E+00 0 0 0 0 

$ 

$=============================== LOAD CURVES =================================== 

$ 

*DEFINE_CURVE 


1 0 .000E+00 .000E+00 .000E+00 .000E+00 

.00000000E+00 .10000000E+01 

.10000000E+01 .10000000E+01 

*END 

Page A.69


Results: 

OASYS D3PLOT: HEMISPHERICAL SHELL 

Displacement 

0.21 

0.18 

0.15 

0.12 

0.09 

0.06 

0.03 

DISP_RESULTANT 

.04 

17.08 

34.12 

51.16 

68.20 

85.24 

102.28 

119.32 

x 1.0E-03 

Z 

Y 

.059998 

0 

0 0.01 0.02 0.03 

Time 

0.04 0.05 0.06 


HEMISPHERICAL SHELL 



Version 7.0 

5-Feb-97 

X 

Page A.70


LS-DYNA Manual Section: *CONTROL_SHELL 

Example of: Twisted Cantilever Beam 

Example Filenames: beam_twist.key 

Description: 

A beam twisted 90 degrees about its length is constrained on one edge and has a point load 

prescribed normal to the opposite end of the beam. 

Model: 

The beam measures 12.00 × 1.10 × 0.32 cubic inches. A concentrated load of 0.1667 pounds is 

applied to each node on the end in both the x and y direction. The calculation terminates at 0.0018 

seconds. 

Input: 

This model uses the Hughes-Liu formulation. The element has the shell normal update calculation 

performed at each nodal fiber every cycle. (*CONTROL_SHELL) 

Results: 

The beam oscillations about a neutral amplitude. 

Reference: 

Belytschko, Wang and Chiang. 

Page A.71



*KEYWORD 

*TITLE 

TWISTED BEAM 

$ 

$================================ CONTROL CARDS ================================ 

$ 




$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ] 

1.800E-02 0 .000E+00 .000E+00 .000E+00 





$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

2.000E+01 2 -2 0 1 2 1 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 .000E+00 0 0 1 0 0 




$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

0 0 0 0 .000E+00 




$ 1 ][ 2 ][ 3 ][ 4 ] 

0 0 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ][ 8 ] 

0 .000E+00 .000E+00 .000E+00 .000E+00 0 .000E+00 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

0 0 0 0 .000E+00 2 1000 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 .000E+00 0 .000E+00 .000E+00 0 0 0 

$ 


$ 


1.800E-02 


1.800E-02 


1.800E-02 

*DATABASE_BNDOUT 

1.800E-02 


5.000E-05 0 1 



1.000E-05 0 


0 


0 


5.000E-05 0 

Page A.72



37 


0 0 4 0 0 0 0 0 

0 0 0 

$ 


$ 

*MAT_ELASTIC 

$ Material 1 : TWISTED BEAM - STEEL 

1 2.000E-04 2.900E+07 .3300 .000E+00 .000E+00 

$ 


$ 


$ Section 1 : TWISTED BEAM - STEEL 

1 0 .00000 4.0 .0 .0 0 

3.200E-01 3.200E-01 3.200E-01 3.200E-01 .000E+00 

$ 


$ 

*PART 

TWISTED BEAM - STEEL 

1 1 1 0 0 0 

$ 

$=================================== NODES ===================================== 

$ 

*NODE 


1 -.55000001E+00 .00000000E+00 .00000000E+00 0 0 

... 

39 .00000000E+00 .55000001E+00 .12000000E+02 0 0 

$ 

$================================== ELEMENTS =================================== 

$ 



1 1 1 4 5 2 

... 

24 1 35 38 39 36 

$ 


$ 



1 1 1 1 1 1 1 1 

2 1 1 1 1 1 1 1 

3 1 1 1 1 1 1 1 


1 .0 .0 .0 1.0 .0 .0 

.0 1.0 .0 

$ 

$================================= CONSTRAINTS ================================= 

$ 

$ 


$ 

$ 


$ 

$ 

$================================== LOADING ==================================== 

$ 



37 2 1 1.667E-01 0 0 0 0 

38 2 1 1.667E-01 0 0 0 0 

39 2 1 1.667E-01 0 0 0 0 

37 2 1 1.667E-01 0 0 0 0 

38 2 1 1.667E-01 0 0 0 0 

39 2 1 1.667E-01 0 0 0 0 

$ 

$=============================== LOAD CURVES =================================== 

$ 

*DEFINE_CURVE 


1 0 .000E+00 .000E+00 .000E+00 .000E+00 

.00000000E+00 .10000000E+01 

.10000000E+04 .10000000E+01 

*END 

Page A.73


Results: 

OASYS D3PLOT: TWISTED BEAM 

Displacement 

14 

12 

10 

8 

6 

4 

DISP_RESULTANT 

.00 

2.00 

4.01 

6.01 

8.01 

10.02 

12.02 

14.02 

x 1.0E-03 

Y 

X 

.018000 

2 

E-3 

0 

0 

E-3 

3 6 9 

Time 

12 15 18 

Disp y - node 37 

TWISTED BEAM 



Version 7.0 

5-Feb-97 

Z 

Page A.74


LS-DYNA Manual Section: *DEFORMABLE_TO_RIGID 

Additional maual Sections: *LOAD_BODY_Y 

Example of: Interaction of Pendulums 

Example Filenames: pendulum_impact.key 

pendulum_impact.key01 

pendulum_impact.key02 

Execution lines: Initial run pendulum_impact.key 

Restart 1 pendulum_impact.key01 + pendulum_impact..dpf01 

Restart 2 pendulum_impact.key02 + pendulum_impact..dpf02 

Description: 

Two cubes are connected by bars to a pendulum. One cube is in a horizontal position with 

gravitational acceleration, base acceleration. The cubes are treated as rigid bodies while no contact 

or deformation occurs. The cubes are flexible during contact. Then, the cubes become rigid again. 

Model: 

Both cubes are modeled as one volume element with side length 10 mm. The elastic material 

describes both cubes and the bars. The distance from the middle of the cube to the bearing shaft 

is 100 mm. The system is subjected to an acceleration of gravity of 10,000 kg mm/second 2 . 

The calculations terminate at 0.5 seconds. 

Input: 

Base acceleration defines gravity (*LOAD_BODY_Y), which is changed in time by a load curve 

(*DEFINE_CURVE). Surface to surface contact type 3 defines the interface between the two cubes 

(*CONTACT_SURFACE_TO_SURFACE). 

The material definition of the cubes changes to a rigid material in the beginning of the calculations 

(*DEFORMABLE_TO_RIGID). 

Reference: 


Page A.75



*KEYWORD 

*TITLE 

RIGID/DEFORMABLE MATERIAL SWITCHING 

$ 

$================================ CONTROL CARDS ================================ 

$ 




$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ] 

1.700E-01 0 1.000E-04 .000E+00 .000E+00 





$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 0 0 0 0 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 .000E+00 0 0 1 0 0 




$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

0 0 0 0 .000E+00 




$ 1 ][ 2 ][ 3 ][ 4 ] 

0 0 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ][ 8 ] 

0 .000E+00 .000E+00 .000E+00 .000E+00 0 .000E+00 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

0 1000 99999 0 .000E+00 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 .000E+00 0 .000E+00 .000E+00 0 0 0 


4 .000E+00 

$ 


$ 


1.000E-03 


1.000E-02 0 1 



1.000E-03 0 


0 


0 


1.000E-02 0 


1 11 


0 0 0 1 0 0 0 0 

Page A.76


0 0 0 

$ 


$ 

*MAT_ELASTIC 

$ Material 1 : SOLID - ELASTIC 

1 7.840E-08 2.100E+05 .3000 .000E+00 .000E+00 

$ 


$ 


$ Section 1 : SOLID - ELASTIC 

1 0 

$------------------------------------------------------------------------------- 

*SECTION_BEAM 

$ Section 2 : BEAM - ELASTIC 

2 3 1.00000 1.0 .0 

1.000E+01 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 

$ 


$ 

*PART 

SOLID - ELASTIC 

1 1 1 0 0 0 

$------------------------------------------------------------------------------- 

*PART 

SOLID - ELASTIC 

2 1 1 0 0 0 

$------------------------------------------------------------------------------- 

*PART 

BEAM - ELASTIC 

3 2 1 0 0 0 


$ pid mrb 

1 


$ pid mrb 

2 

$ 

$=================================== NODES ===================================== 

$ 

*NODE 


1 -.95000000E+02 .10500000E+03 .00000000E+00 0 0 

... 

20 .15000000E+02 .10000000E+03 .60000000E+02 0 0 

$ 

$================================== ELEMENTS =================================== 

$ 



1 1 1 2 4 3 5 6 8 7 

2 2 11 12 14 13 15 16 18 17 

*ELEMENT_BEAM 

$ ID PART NODE 1 NODE 2 NODE 3 

1 3 3 9 1 

... 

8 3 18 20 1 

$ 


$ 



9 1 1 1 1 0 0 0 

10 1 1 1 1 0 0 0 

19 1 1 1 1 0 0 0 

20 1 1 1 1 0 0 0 


1 .0 .0 .0 1.0 .0 .0 

.0 1.0 .0 

$ 

$================================= CONSTRAINTS ================================= 

$ 

$ 


$ 

$ 


$ 

$ 

$================================== LOADING ==================================== 

Page A.77


$ 

*LOAD_BODY_Y 

$ CURVE ID FACTOR DR LC X CENTER Y CENTER Z CENTER 

1 1.000E+04 0 .0 .0 .0 

$ 


$ 


$ NUMBER NAME 

1 Contact # 1 


1 2 0 0 0 0 0 0 


.000E+00 .000E+00 .000E+00 .000E+00 .000E+00 0 .000E+00 .000E+00 


.000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 


0 .000E+00 0 .000E+00 .000E+00 0 0 0 


.000E+00 0 0 

*SET_SEGMENT 

1 .000E+00 .000E+00 .000E+00 .000E+00 

2 6 8 4 .000E+00 .000E+00 .000E+00 .000E+00 

*SET_SEGMENT 

2 .000E+00 .000E+00 .000E+00 .000E+00 

11 15 17 13 .000E+00 .000E+00 .000E+00 .000E+00 

$ 

$=============================== LOAD CURVES =================================== 

$ 

*DEFINE_CURVE 


1 0 .000E+00 .000E+00 .000E+00 .000E+00 

.00000000E+00 .10000000E+01 

.10000000E+04 .10000000E+01 

*END 

1st Restart: 

*KEYWORD 

*TITLE 


$ 

$================================ CONTROL CARDS ================================ 

$ 




$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ] 

1.800E-01 0 .000E+00 .000E+00 .000E+00 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 1.000E-01 0 .000E+00 .000E+00 0 0 0 

$ 


$ 


1.000E-03 

*RIGID_DEFORMABLE_R2D 

$ PART ID 1 

*RIGID_DEFORMABLE_R2D 

$ PART ID 2 

*END 

Page A.78


2nd Restart: 

*KEYWORD 

*TITLE 


$ 

$================================ CONTROL CARDS ================================ 

$ 




$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ] 

5.000E-01 0 .000E+00 .000E+00 .000E+00 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 9.000E-01 0 .000E+00 .000E+00 0 0 0 

$ 


$ 


1.000E-03 

*RIGID_DEFORMABLE_D2R 

$ PART ID 1 

*RIGID_DEFORMABLE_D2R 

$ PART ID 2 

*END 

Page A.79


Results: 

EFORMABLE MATERIAL SWITCHING 

EFORMABLE MATERIAL SWITCHING 

Y 

Z 

X 

.000000000 

Y 

Z 

.349999 

X 

OASYS D3PLOT: RIGID/DEFORMABLE MATERIAL SWITCHING 

OASYS D3PLOT: RIGID/DEFORMABLE MATERIAL SWITCHING 

Page A.80


Time 

Displacement 

6 

5 

4 

3 

2 

1 

E-5 

0 

0 0.1 0.2 0.3 0.4 0.5 

Time 

Time step 

80 

60 

40 

20 

0 

-20 

-40 

-60 

-80 

-100 




Version 7.0 

5-Feb-97 

0 0.1 0.2 0.3 0.4 0.5 

Time 

Material 1 - y Displacement 

Material 2 - y Displacement 




Version 7.0 

5-Feb-97 

Page A.81


LS-DYNA Manual Section: *INTEGRATION_SHELL 

Example of: Cantilever Beam with Lobotto Integration 

Example File Name: beam_lobotto.key 

Description: 

A cantilever beam is loaded by a concentrated nodal load. The load is then removed and the beam 

vibration is critically damped. Lobotto integration rules place the quadrature points on the true 

surfaces on the shell. [See Hughes]. 

Model: 

The plate measures 1.00 × 0.10 × 0.01 in 3 and is modeled with 60 Belytschko-Tsay shell elements. 

The displacement of the nodes is fixed at one end and a concentrated load of 0.05 pounds is applied 

to the other end. Symmetry conditions for the plane strain case exist on the beam sides. The 

termination time is 0.01 seconds plus the period of the beam. 

Input: 

The concentrated loads and load curve definition 1 define the load on the end of the beam 

(*LOAD_NODE_POINT, *DEFINE_CURVE). The beam is critically damped 

(*DAMPING_GLOBAL) The number of integration points is 5 (*SECTION_SHELL). The shell 

integration rule is the Lobotto integration rule (*SECTION_SHELL) 

Results: 

The displacement of the beam damps out critically. The x-stress values at the integration points 

exhibit tension on one side, compression on the opposite side, and balance at the neutral axis. 

Page A.82



*KEYWORD 

*TITLE 

LOBOTTO INTEGRATION 

$ 

$================================ CONTROL CARDS ================================ 

$ 




$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ] 

1.534E-02 0 .000E+00 .000E+00 .000E+00 





$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 0 0 0 0 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 .000E+00 0 0 1 0 0 




$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

0 0 0 0 .000E+00 




$ 1 ][ 2 ][ 3 ][ 4 ] 

2 0 1 1 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ][ 8 ] 

0 .000E+00 .000E+00 .000E+00 .000E+00 0 .000E+00 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

0 0 0 0 .000E+00 2 1000 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 .000E+00 0 .000E+00 .000E+00 0 0 0 

$ 


$ 


1.000E-04 


1.000E-04 


1.000E-04 


3.068E-04 0 1 



1.000E-04 0 


0 


0 


3.068E-04 0 


31 

Page A.83



1 


0 0 5 0 0 0 0 0 

0 0 0 

$ 


$ 


$ Material 1 : CANTILEVER BEAM - ALUMINUM 

1 7.850E-04 1.000E+07 .3000 2.000E+04 1.000E+05 1.000E+00 

.000E+00 .000E+00 .000E+00 

$ 


$ 


$ Section 1 : CANTILEVER BEAM - ALUMINUM 

1 0 .00000 5.0 .0 -1.0 0 

1.000E-02 1.000E-02 1.000E-02 1.000E-02 .000E+00 

*INTEGRATION_SHELL 

$ RULE ID POINTS SPACING 

1 5 

$ COORD WEIGHT PART ID 

-1.000E+00 1.000E-01 

-6.546E-01 5.444E-01 

0.000E+00 7.111E-01 

6.546E-01 5.444E-01 

1.000E+00 1.000E-01 

$ 


$ 

*PART 

CANTILEVER BEAM - ALUMINUM 

1 1 1 0 0 0 

$ 

$=================================== NODES ===================================== 

$ 

*NODE 


1 .00000000E+00 .00000000E+00 .00000000E+00 0 0 

... 

93 .10000000E+01 .10000000E+00 .00000000E+00 0 0 

$ 

$================================== ELEMENTS =================================== 

$ 



1 1 1 32 33 2 

... 

60 1 61 92 93 62 

*DAMPING_GLOBAL 

2 .000E+00 

$ 


$ 



1 1 1 1 1 1 1 1 

... 

93 1 0 1 0 1 0 1 


1 .0 .0 .0 1.0 .0 .0 

.0 1.0 .0 

$ 

$================================= CONSTRAINTS ================================= 

$ 

$ 


$ 

$ 


$ 

$ 

$================================== LOADING ==================================== 

$ 



31 3 1-1.000E+00 0 0 0 0 

62 3 1-1.000E+00 0 0 0 0 

93 3 1-1.000E+00 0 0 0 0 

$ 

Page A.84


$=============================== LOAD CURVES =================================== 

$ 

*DEFINE_CURVE 


1 0 .000E+00 .000E+00 .000E+00 .000E+00 

.00000000E+00 .00000000E+00 

.80000004E-02 .16670000E-02 

.15340000E-01 .16670000E-02 

*DEFINE_CURVE 


2 0 .000E+00 .000E+00 .000E+00 .000E+00 

.00000000E+00 .00000000E+00 

.80000004E-02 .00000000E+00 

.99999998E-02 .23530000E+04 

.15340000E-01 .23530000E+04 

*END 

Page A.85


Results: 

OASYS D3PLOT: LOBOTTO INTEGRATION 

Displacement 

0 

-4 

-8 

-12 

-16 

-20 

Z_DISPLACEMENT 

-18.20 

-15.60 

-13.00 

-10.40 

-7.80 

-5.20 

-2.60 

.00 

x 1.0E-03 

Y 

Z 

.015340 

-24 

E-3 

-28 

0 

E-3 

2 4 6 8 

Time 

10 12 14 16 


LOBOTTO INTEGRATION 



Version 7.0 

5-Feb-97 

X 

Page A.86


LS-DYNA Manual Section: *LOAD_BODY_GENERALIZED 

Additional Sections: *DEFINE_CURVE 


Example of: Rotating Elements 

Example Filename: shell_global.key 

Description: 

A body has constant angular velocity. The radial vibration introduced due to the rapid deployment 

of the rotation is damped out in the initialization phase using dynamic relaxation. 

Model: 

The body measures 200 × 100 × 10 mm 3 . The body consists of 2 Belytschko-Tsay elastic shell 

elements. The body rotates about the y-axis at 62.83 radians per second. The analysis ends at 0.1 

seconds. 

Input: 

All nodes have an initial translational velocity based on the angular velocity v=omega x r. 

(*LOAD_BODY_GENERALIZED, *DEFINE_CURVE). Dynamic relaxation damps oscillations 

in the radial direction during the initialization. This essentially pre-stresses the structure and the 

load continues into the analysis portion. (*LOAD_BODY_GENERALIZED) 

Because of the condition of constant angular velocity of the two nodes on the axis of rotation, the 

motion remains uniform throughout the calculation (*INITIAL_VELOCITY_NODE). 

Reference: 


Page A.87



*KEYWORD 

*TITLE 

MASS WITH ANGULAR ROTATION - 2 SHELL ELEMENTS 

$ 

$================================ CONTROL CARDS ================================ 

$ 




$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ] 

1.000E-01 0 .000E+00 .000E+00 .000E+00 





$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 0 0 0 0 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 .000E+00 0 0 1 0 0 




$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

0 0 0 0 .000E+00 




$ 1 ][ 2 ][ 3 ][ 4 ] 

0 0 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ][ 8 ] 

0 .000E+00 .000E+00 .000E+00 .000E+00 0 .000E+00 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

0 0 0 0 .000E+00 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 .000E+00 0 .000E+00 .000E+00 0 0 0 


4 .000E+00 

$ 


$ 


1.000E-03 


1.000E-02 0 1 



5.000E-04 0 


0 


0 


1.000E-02 0 


1 2 3 4 5 6 


1 2 

Page A.88



0 0 0 0 0 0 0 0 

0 0 0 



1 0 0 1 0 0 


1 

1 2 


1 

1 

$ 


$ 

*MAT_ELASTIC 

$ Material 1 : SHELLS 

1 1.000E-08 2.100E+05 .3000 .000E+00 .000E+00 

$ 


$ 


$ Section 1 : SHELLS 

1 0 .00000 3.0 .0 .0 0 

1.000E+01 1.000E+01 1.000E+01 1.000E+01 .000E+00 

$ 


$ 

*PART 

SHELLS 

1 1 1 0 0 0 

$ 

$=================================== NODES ===================================== 

$ 

*NODE 


1 .00000000E+00 .00000000E+00 .00000000E+00 0 0 

... 

6 .20000000E+03 .10000000E+03 .00000000E+00 0 0 

$ 

$================================== ELEMENTS =================================== 

$ 



1 1 1 3 4 2 

2 1 3 5 6 4 

$ 


$ 



1 1 1 1 1 0 0 0 

2 1 1 0 1 0 0 0 


1 .0 .0 .0 1.0 .0 .0 

.0 1.0 .0 



1 6 0 1 1.000E+00 0 .000E+00 

2 6 0 1 1.000E+00 0 .000E+00 

$ 

$================================= CONSTRAINTS ================================= 

$ 


$ 


1 .000E+00 .000E+00 .000E+00 .000E+00 6.283E+01 .000E+00 

... 

6 .000E+00 .000E+00-1.257E+04 .000E+00 6.283E+01 .000E+00 

$ 

$================================== LOADING ==================================== 

$ 

$=============================== LOAD CURVES =================================== 

$ 

*DEFINE_CURVE 


1 0 .000E+00 .000E+00 .000E+00 .000E+00 

.00000000E+00 .62830002E+02 

.10000000E+01 .62830002E+02 

*END 

Page A.89


Results: 

OASYS D3PLOT: MASS WITH ANGULAR ROTATION - 2 SHELL ELE 

Displacement 

15 

10 

5 

0 

-5 

VELOCITY vector 

.00 

2.09 

4.19 

6.28 

8.37 

10.47 

12.56 

x 1.0E+03 

Z 

Y 

.019983 

-10 

E3 

-15 

0 0.02 0.04 0.06 0.08 0.10 

Time 

Vel x - node 4 

Vel x - node 6 

MASS WITH ANGULAR ROTATION - 2 SHELL ELE 



Version 7.0 

5-Feb-97 

X 

Page A.90


LS-DYNA Manual Section: *MAT_PIECEWISE_LINEAR_PLASTICITY 

Example of: Piecewise Linear Plasticity Fragmenting Plate 

Example File Name: plate_shatter.key 

Description: 

A plate of 1,200 Belytschko-Tsay shell elements strikes a stonewall at an angle of 45 degrees from 

the stonewall normal. The impact velocity is 20,775 in/sec. and the termination time is 0.00025 

seconds. 

Model: 

The material description contains Young’s Modulus, Poisson’s ratio, yield stress, load curve for 

strain rate, hardening modulus, ultimate plastic strain, and time step size for element deletion. 

Input: 

The material definition for the Belytschko-Tsay shell uses a viscous hourglass control 

(*CONTROL_HOURGLASS). The Young’s Modulus, Poisson’s ratio, yield stress and hardening 

modulus are 16 Msi, 0.34, 15,500 psi, and 192,000 psi respectively. The plastic strain is 32% and 

the minimum time step size is 0.3 mseconds. 

Results: 

The plate deforms away from the stonewall and the plate fragments. 

Page A.91



*KEYWORD 

*TITLE 

TEST FOR MATERIAL 24 WITH FAILURE 

$ 

$================================ CONTROL CARDS ================================ 

$ 




$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ] 

2.500E-04 0 5.000E-02 .000E+00 .000E+00 





$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 0 0 0 0 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

1.000E-02 .000E+00 0 0 1 0 0 




$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

0 0 0 0 .000E+00 




$ 1 ][ 2 ][ 3 ][ 4 ] 

0 0 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ][ 8 ] 

0 .000E+00 .000E+00 .000E+00 .000E+00 0 .000E+00 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

0 0 0 0 .000E+00 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 .000E+00 0 .000E+00 .000E+00 0 0 0 


4 .000E+00 

$ 


$ 


1.250E-05 0 1 



1.000E-06 0 


0 


0 


1.250E-05 0 


0 0 0 0 0 0 0 0 

0 0 0 

$ 


$ 

Page A.92


*MAT_PIECEWISE_LINEAR_PLASTICITY 

$ Material 1 : PLATE - TITANIUM 

1 4.141E-04 1.600E+07 .3500 1.550E+05 1.920E+05 3.200E-01 3.000E-08 

.000E+00 .000E+00 .0 .0 

.000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 

.000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 

$ 


$ 


$ Section 1 : PLATE - TITANIUM 

1 0 .00000 5.0 3.0 .0 0 

1.250E-01 1.250E-01 1.250E-01 1.250E-01 .000E+00 

$ 


$ 

*PART 

PLATE - TITANIUM 

1 1 1 0 0 0 

$------------------------------------------------------------------------------- 

*PART 


2 1 1 0 0 0 

$------------------------------------------------------------------------------- 

*PART 


3 1 1 0 0 0 

$ 

$=================================== NODES ===================================== 

$ 

*NODE 


1 .00000000E+00 .00000000E+00 .00000000E+00 0 0 

... 1285 -.50000001E-01 -.10000000E+02 .50000000E+01 0 0 

$ 

$================================== ELEMENTS =================================== 

$ 



1 2 22 1 2 23 

.. 1201 3 1282 1283 1284 1285 

$ 


$ 



1282 1 1 1 1 1 1 1 

1283 1 1 1 1 1 1 1 

1284 1 1 1 1 1 1 1 

1285 1 1 1 1 1 1 1 


1 .0 .0 .0 1.0 .0 .0 

.0 1.0 .0 

$ 

$================================= CONSTRAINTS ================================= 

$ 

$ 


$ 

$ 


$ 


0 1 0 

-1.469E+04-1.469E+04 .000E+00 .000E+00 .000E+00 .000E+00 

.000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 


1 

1281 1282 1283 1284 1285 

$ 

$================================== LOADING ==================================== 

$ 

$ 


$ 


$ NUMBER NAME 

1 Contact # 1 


Page A.93


1 2 0 0 0 0 1 1 


3.000E-01 3.000E-01 .000E+00 .000E+00 .000E+00 0 .000E+00 .000E+00 


.000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 


0 .000E+00 0 .000E+00 .000E+00 0 0 0 


.000E+00 0 0 

*SET_SEGMENT 

1 .000E+00 .000E+00 .000E+00 .000E+00 

22 1 2 23 .000E+00 .000E+00 .000E+00 .000E+00 

... 

1280 1259 1260 1281 .000E+00 .000E+00 .000E+00 .000E+00 

*SET_SEGMENT 

2 .000E+00 .000E+00 .000E+00 .000E+00 

1282 1283 1284 1285 .000E+00 .000E+00 .000E+00 .000E+00 

*END 

Page A.94


Results: 

OASYS D3PLOT: TEST FOR MATERIAL 24 WITH FAILURE 

OASYS D3PLOT: TEST FOR MATERIAL 24 WITH FAILURE 

Z 

Y 

X 

.000000000 

Z 

Y 

.000250 

X 

Page A.95


LS-DYNA Manual Section: *MAT_RIGID 

Additonal Sections: *DEFINE_COORDINATE_VECTOR 

Example of: Rigid Sliding Block in Local Coordinate System 

Example File Name: block_slide.key 

Description: 

A center of mass is constrained to slide along a local coordinate system. The termination time is 

0.010 seconds. 

Model: 

The material description references a local coordinate system to constrain the rigid block. The rigid 

block is free to translate along the local z axis. 

Input: 

The material definition is a rigid material (*MAT_RIGID). The material specifies the use of a 

referece local coordinate system, the local coordinate constrait value of 100111 (tx ty tz rx ry rz), 

and the local coordinate system for output. The local coordinate system specifies that the local 

origin si the global origin, the local x-axis point s (1.0,0.0,1.0) and the local y-axis point is 

(0.0,0.0,1.0) (*DEFINE_COORDINATE_VECTOR). 

Results: 

The block slides along the local coordinate system. 

Page A.96



*KEYWORD 

*TITLE 

SLIDING BLOCK 

$ 

$================================ CONTROL CARDS ================================ 

$ 




$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ] 

1.000E-02 0 .000E+00 .000E+00 .000E+00 





$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 0 0 0 0 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 .000E+00 0 0 1 0 0 




$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

0 0 0 0 .000E+00 




$ 1 ][ 2 ][ 3 ][ 4 ] 

0 0 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ][ 8 ] 

0 .000E+00 .000E+00 .000E+00 .000E+00 0 .000E+00 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

0 0 0 0 .000E+00 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 .000E+00 0 .000E+00 .000E+00 0 0 0 

$ 


$ 


5.000E-04 0 1 



.000E+00 0 


0 


0 


5.000E-04 0 


0 0 0 0 0 0 0 0 

0 0 0 

$ 


$ 

*MAT_RIGID 

$ Material 1 : BLOCK 

Page A.97


1 7.850E-04 3.000E+07 .3000 .0 .0 .0 

-1.0 1.0 100111.0 

1.000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 

$------------------------------------------------------------------------------- 

*MAT_ELASTIC 

$ Material 2 : PLATE 

2 7.850E-04 3.000E+07 .3000 .000E+00 .000E+00 

$ 


$ 


$ Section 1 : BLOCK 

1 0 

$------------------------------------------------------------------------------- 


$ Section 2 : PLATE 

2 0 .00000 .0 .0 .0 0 

1.000E+00 1.000E+00 1.000E+00 1.000E+00 .000E+00 

$ 


$ 

*PART 

BLOCK 

1 1 1 0 0 0 

$------------------------------------------------------------------------------- 

*PART 

PLATE 

2 2 2 0 0 0 

$ 

$=================================== NODES ===================================== 

$ 

*NODE 


1 .00000000E+00 .00000000E+00 .00000000E+00 0 0 

... 

68 .10000000E+01 .10000000E+01 -.10000000E+01 0 0 

$ 

$================================== ELEMENTS =================================== 

$ 



1 1 1 2 6 5 17 18 22 21 

... 

27 1 43 44 48 47 59 60 64 63 



1 2 65 67 68 66 

$ 


$ 

*DEFINE_COORDINATE_VECTOR 

1 1.000E+00 .000E+00 1.000E+00 .000E+00 .000E+00 1.000E+00 

$ 

$================================= CONSTRAINTS ================================= 

$ 

$ 


$ 

$ 

$================================== LOADING ==================================== 

$ 

*LOAD_SEGMENT 


1 1.000E+00 .000E+00 53 49 50 54 

1 1.000E+00 .000E+00 57 53 54 58 

1 1.000E+00 .000E+00 61 57 58 62 

1 1.000E+00 .000E+00 54 50 51 55 

1 1.000E+00 .000E+00 58 54 55 59 

1 1.000E+00 .000E+00 62 58 59 63 

1 1.000E+00 .000E+00 55 51 52 56 

1 1.000E+00 .000E+00 59 55 56 60 

1 1.000E+00 .000E+00 63 59 60 64 

$ 

$=============================== LOAD CURVES =================================== 

$ 

*DEFINE_CURVE 


1 0 .000E+00 .000E+00 .000E+00 .000E+00 

.00000000E+00 .10000000E+03 

.99999998E-02 .10000000E+03 

*END 

Page A.98


Results: 

OASYS D3PLOT: SLIDING BLOCK 

OASYS D3PLOT: SLIDING BLOCK 


Deformable Element for Timestep Control 

Z 

Y 

.004998 

Z 

Y 

.009996 

X 

X 

Page A.99


LS-DYNA Manual Section: *MAT_SPRING 

Additional Sections: *BOUNDARY_PRESCRIBED_MOTION 


*CONSTRAINED_JOINT_SPHERICAL 

*LOAD_BODY_Z 

*PART_INERTIA 

Example of: Belted Dummy with Springs 

Example Filename: dummy_belted.key 

Description: 

This is a simulation of the interaction between a dummy and seating system. The dummy has an 

initial velocity, base vehicle acceleration, and decelerated base. 

Model: 

The dummy consists of 15 ellipsoidal rigid bodies connected through cylindrical joints, springs and 

dampers. The base of the seat belts and the seat decelerates backwards relative to the dummy. The 

termination of the calculation is 12. 

Input: 

The dummy consists of rigid bodies 1 through 15 (*MAT_RIGID). Materials 16 through 20 define 

the seat and material 21 and 22 define the seat belt. The rigid bodies are constrained with respect 

to each other with spherical joints (*CONSTRAINED_JOINT_SPHERICAL). Discrete springs and 

dampers between the rigid body provide the relative stiffness and viscosity 

(*ELEMENT_DISCRETE). The initial velocity of all nodes is 14.8 units 

(*INITIAL_VELOCITY_NODE), while the acceleration of the seat and belt ends follow an 

acceleration curve in the opposite direction. (*DEFINE_CURVE) Load curve 51 defines the base 

acceleration (*LOAD_BODY_Z). 

Results: 

LS-DYNA predicts that the dummy slides under the seat belts. 

Reference: 

Stillman, D. W. 

Page A.100



*KEYWORD 

*TITLE 

BELTED DUMMY 

$ 

$================================ CONTROL CARDS ================================ 

$ 




$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ] 

1.200E-01 0 .000E+00 .000E+00 .000E+00 





$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 0 0 0 0 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 .000E+00 0 0 1 0 2 




$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

0 0 0 0 .000E+00 




$ 1 ][ 2 ][ 3 ][ 4 ] 

0 0 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ][ 8 ] 

0 .000E+00 .000E+00 .000E+00 8.000E-01 0 .000E+00 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

0 0 0 0 .000E+00 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 8.000E-01 0 .000E+00 .000E+00 0 0 0 

$ 


$ 


2.500E-03 0 1 



.000E+00 0 


0 


0 


2.500E-03 0 


0 0 0 0 0 0 0 0 

0 0 0 

$ 


$ 

*MAT_RIGID 

$ Material 1 : MATERIAL TYPE # (RIGID) 

Page A.101


1 4.064E+03 4.000E+08 .3000 .0 .0 .0 

.0 .0 .0 

.000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 

... 

*MAT_ELASTIC 

$ Material 22 : 

22 4.000E+03 2.000E+08 .3000 .000E+00 .000E+00 

... 

*MAT_SPRING_NONLINEAR_ELASTIC 

$ Material 101 : SPRING 101 

101 1 0 

... 

*MAT_DAMPER_NONLINEAR_VISCOUS 

$ Material 208 : SPRING 208 

208 49 

$ 


$ 


$ Section 1 : MATERIAL TYPE # (RIGID) 

1 0 .00000 .0 .0 .0 0 

1.000E-02 1.000E-02 1.000E-02 1.000E-02 .000E+00 

... 

*SECTION_DISCRETE 

$ Section 208 : SPRING 208 

208 1 .000E+00 .000E+00 .000E+00 .000E+00 

.000E+00 .000E+00 

$ 


$ 

*PART_INERTIA 

MATERIAL TYPE # (RIGID) 

1 1 1 0 0 0 

-1.739E-01 .000E+00 6.523E-01 4.535E+00 0 

1.590E-02 .000E+00 1.424E-04 2.400E-02 .000E+00 2.210E-02 

1.480E+01 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 

... 

*PART 

SPRING 208 

208 208 208 0 0 

$ 

$=================================== NODES ===================================== 

$ 

*NODE 


1 -.24169317E+00 -.32869909E-01 .58760071E+00 0 0 

... 2043 -.58595401E+00 .28587806E+00 .61651736E+00 0 0 

$ 

$================================== ELEMENTS =================================== 

$ 



1 1 1 4 5 2 

... 1950 22 404 367 369 379 


$ ID PART NODE 1 NODE 2 OR VEC SCALE FACTOR PRINT OFFSET 

1 101 1 129 1 .0000E+00 1 .0000E+00 

... 108 208 1505 1675 40 .0000E+00 1 .0000E+00 

*DEFINE_SD_ORIENTATION 

$ ID TYPE X VEC Y VEC Z VEC NODE 1 NODE 2 

1 2 .000E+00 .000E+00 .000E+00 100 229 

... 

42 2 .000E+00 .000E+00 .000E+00 1586 1736 

$ 


$ 



1763 1 0 1 1 1 1 1 

... 

2043 1 0 1 1 0 0 0 


1 .0 .0 .0 1.0 .0 .0 

.0 1.0 .0 



1763 1 1 50-1.000E+00 0 .000E+00 

... 

Page A.102


2043 1 1 50-1.000E+00 0 .000E+00 

$ 

$================================= CONSTRAINTS ================================= 

$ 



1 1 


1 

99 100 101 102 

... 



15 15 


15 

1733 1734 1735 1736 

*CONSTRAINED_JOINT_SPHERICAL 

$ NODE 1 NODE 2 STIFFNESS 

99 227 .000E+00 

... 

1580 1733 .000E+00 

$ 


$ 

$ 


$ 


1 1.480E+01 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 

... 

2043 1.480E+01 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 

$ 

$================================== LOADING ==================================== 

$ 

*LOAD_BODY_Z 

$ CURVE ID FACTOR DR LC X CENTER Y CENTER Z CENTER 

51-1.000E+00 0 .0 .0 .0 

$ 


$ 


$ NUMBER NAME 

1 Contact # 1 


1 2 0 0 0 0 0 0 


6.200E-01 .000E+00 .000E+00 .000E+00 .000E+00 0 .000E+00 .000E+00 


.000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 


0 .000E+00 0 .000E+00 .000E+00 0 0 0 


.000E+00 0 0 

*SET_SEGMENT 

1 .000E+00 .000E+00 .000E+00 .000E+00 

1780 1783 1784 1781 4.000E+00 .000E+00 .000E+00 .000E+00 

... 

1784 1787 1788 1785 4.000E+00 .000E+00 .000E+00 .000E+00 

*SET_SEGMENT 

2 .000E+00 .000E+00 .000E+00 .000E+00 

1 4 5 2 1.320E+02 .000E+00 .000E+00 .000E+00 

... 

311 314 315 312 1.320E+02 .000E+00 .000E+00 .000E+00 

$ 

$=============================== LOAD CURVES =================================== 

$ 

*DEFINE_CURVE 


1 0 .000E+00 .000E+00 .000E+00 .000E+00 

-.17100000E+01 -.53800000E+03 

... 

.17100000E+01 .53800000E+03 

*END 

Page A.103


Results: 

OASYS D3PLOT: BELTED DUMMY 

OASYS D3PLOT: BELTED DUMMY 

Z 

Y 

X 

.000000000 

Z 

.119996 

Y 

X 

Page A.104


LS-DYNA Manual Section: *RIGIDWALL_GEOMETRIC_SPHERE_MOTION 

Example of: Geometric spherical rigidwall impacts a plate. 

Example Filename: sphere_rigidwall.key 

Description: 

A “Stonewall” sphere impacts an elastic plate. (The stonewall will be shown in D3PLOT but will 

not appear to move.) 

Model: 

The plate has an elastic material model with Belytschko-Tsay shell formulation. The plate is 40 × 

40 × 2 mm 3 . The sphere has a radius of 8 mm and its center is 9 mm above the plate. The sphere 

moves towards the plate with a prescribed velocity of 3 mm/second. Termination time is set to 

0.0005 seconds. 

Input: 

A spherical stonewall surface represents the true geometry of the ball. 

(*RIGIDWALL_GEOMETRIC_SPHERE_MOTION). The stone wall cards contain direction and 

load curve number (*DEFINE_LOAD). The box option defines the nodes that intercat with the 

stonewall definition. 

Reference: 


Page A.105



*KEYWORD 

*TITLE 

SPHERICAL GEOMETRIC RIGIDWALL 

$ 

$================================ CONTROL CARDS ================================ 

$ 




$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ] 

5.000E-04 0 .000E+00 .000E+00 .000E+00 





$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 0 0 0 0 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 .000E+00 0 0 1 0 0 




$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

0 0 0 0 .000E+00 




$ 1 ][ 2 ][ 3 ][ 4 ] 

0 0 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ][ 8 ] 

0 .000E+00 .000E+00 .000E+00 .000E+00 0 .000E+00 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

0 0 0 0 .000E+00 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 .000E+00 0 .000E+00 .000E+00 0 0 0 


4 .000E+00 

$ 


$ 


2.000E-05 0 1 



1.000E-07 0 


0 


0 


2.000E-05 0 


0 0 0 1 0 0 0 0 

0 0 0 

$ 


$ 

Page A.106


*MAT_ELASTIC 

$ Material 1 : ELASTIC 

1 2.000E-08 1.000E+05 .3000 .000E+00 .000E+00 

$ 


$ 


$ Section 1 : ELASTIC 

1 0 .83330 2.0 3.0 .0 0 

2.000E+00 2.000E+00 2.000E+00 2.000E+00 .000E+00 

$ 


$ 

*PART 

ELASTIC 

1 1 1 0 0 0 

$ 

$=================================== NODES ===================================== 

$ 

*NODE 


1 .00000000E+00 .00000000E+00 .00000000E+00 0 0 

... 

81 .40000000E+02 .40000000E+02 .00000000E+00 0 0 

$ 

$================================== ELEMENTS =================================== 

$ 



1 1 1 2 11 10 

... 

64 1 71 72 81 80 

$ 


$ 



1 1 0 0 1 0 0 0 

... 

81 1 0 0 1 0 0 0 


1 .0 .0 .0 1.0 .0 .0 

.0 1.0 .0 

$ 

$================================= CONSTRAINTS ================================= 

$ 

$ 


$ 

*RIGIDWALL_GEOMETRIC_SPHERE_MOTION 

0 0 1 


2.000E+01 2.000E+01 9.000E+00 2.000E+01 2.000E+01 .000E+00 .000E+00 

8.000E+00 .000E+00 

1 1 .000E+00 .000E+00-1.000E+00 

*DEFINE_BOX 

1 .000E+00 4.000E+01 .000E+00 4.000E+01-1.000E+00 1.000E+00 

$ 


$ 

$ 

$================================== LOADING ==================================== 

$ 

$ 

$=============================== LOAD CURVES =================================== 

$ 

*DEFINE_CURVE 


1 0 .000E+00 .000E+00 .000E+00 .000E+00 

.00000000E+00 .00000000E+00 

.50000002E-03 .15000000E+02 

*END 

Page A.107


Results: 

OASYS D3PLOT: SPHERICAL GEOMETRIC RIGIDWALL 

OASYS D3PLOT: SPHERICAL GEOMETRIC RIGIDWALL 

Z 

Y 

X 

.000000000 

Z 

Y 

.000279 

X 

Page A.108


Force 

45 

40 

35 

30 

25 

20 

15 

10 

5 

0 

E4 

-5 

0 1 2 3 4 5 

E-4 

Time 

Normal force - wall 1 

SPHERICAL GEOMETRIC RIGIDWALL 



Version 7.0 

7-Feb-97 

Page A.109


LS-DYNA Manual Section: *RIGIDWALL_PLANAR_FORCES 

Example of: Cube Rebounding from a Rigidwall 

Example Filename: rigidwall_cube.key 

Description: 

A cube impacts and rebounds from a rigid plate modelled using a Stonewall (Rigidwall). The 

rigidwall is defined using four nodes si that it appears as a finite rigidwall in D3PLOT. 

Model: 

The cube measures 10 × 10 × 10 mm 3 and is 10 mm above the rigid plate. It has 8 brick elements 

with elastic material properties. The initial velocity of the cube is 100,000 mm/second. The plate 

is an infinite “Stonewall” surface. Termination time is 0.0004 seconds. 

Input: 

The box option defines the nodes with the initial velocity (*INITIAL_VELOCITY. The location 

of the “Stonewall” is at z=0 (*RIGIDWALL_PLANAR_FORCES). The nine nodes on the lower 

side of the cube are slave nodes to the “Stonewall” definition. These slave nodes will not pass this 

plane within 10 time steps by the contact with the “stonewall”. 

Reference: 


Page A.110



*KEYWORD 

*TITLE 

STONEWALL SURFACE 

$ 

$================================ CONTROL CARDS ================================ 

$ 




$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ] 

4.001E-04 0 .000E+00 .000E+00 .000E+00 





$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 0 0 0 0 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 .000E+00 0 0 1 0 0 




$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

0 0 0 0 .000E+00 




$ 1 ][ 2 ][ 3 ][ 4 ] 

2 0 1 1 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ][ 8 ] 

0 .000E+00 .000E+00 .000E+00 .000E+00 0 .000E+00 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

0 1000 0 0 2.000E-06 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 .000E+00 0 .000E+00 .000E+00 0 0 0 


4 .000E+00 

$ 


$ 


2.000E-05 0 1 



1.000E-07 0 


0 


0 


2.000E-05 0 


13 201 


0 0 0 1 0 0 0 0 

0 0 0 


Page A.111


$ 

*MAT_ELASTIC 

$ Material 1 : IMPACTED 

1 2.000E-08 1.000E+05 .3000 .000E+00 .000E+00 

$------------------------------------------------------------------------------- 

*MAT_ELASTIC 

$ Material 2 : IMPACTOR 

2 1.000E-08 1.000E+05 .3000 .000E+00 .000E+00 

$ 


$ 


$ Section 1 : IMPACTED 

1 0 .83330 2.0 3.0 .0 0 

2.000E+00 2.000E+00 2.000E+00 2.000E+00 .000E+00 

$------------------------------------------------------------------------------- 


$ Section 2 : IMPACTOR 

2 0 

$ 


$ 

*PART 

IMPACTED 1 1 1 0 0 0 

$------------------------------------------------------------------------------- 

*PART 

IMPACTOR 2 2 2 0 0 0 

$ 

$=================================== NODES ===================================== 

$ 

*NODE 


1 .00000000E+00 .00000000E+00 .00000000E+00 0 0 

... 227 .25000000E+02 .25000000E+02 .20000000E+02 0 0 

$ 

$================================== ELEMENTS =================================== 

$ 



101 2 201 202 205 204 210 211 214 213 

... 108 2 214 215 218 217 223 224 227 226 

$ 


$ 



1 1 1 1 1 0 0 0 

4 1 1 1 1 0 0 0 

16 1 1 1 1 0 0 0 


1 .0 .0 .0 1.0 .0 .0 

$ 


$ 

*RIGIDWALL_PLANAR_FORCES 

1 0 0 


2.000E+01 2.000E+01 .000E+00 2.000E+01 2.000E+01 1.000E+02 .000E+00 

$ # CYCLES SET ID NODE 1 NODE 2 NODE 3 NODE 4 

10 0 1 4 13 16 


1 

201 202 203 204 205 206 207 208 

209 

$ 


$ 


0 0 1 

.000E+00 .000E+00-1.000E+05 .000E+00 .000E+00 .000E+00 

*DEFINE_BOX 

1 1.490E+01 2.510E+01 1.490E+01 2.510E+01 9.000E+00 2.100E+01 

$ 

$================================== LOADING ==================================== 

$ 

*END 

Page A.112


Results: 

OASYS D3PLOT: STONEWALL SURFACE 



.00 

16.67 

33.33 

50.00 

66.67 

83.33 

100.00 

x 1.0E+03 

.00 

15.53 

31.07 

46.60 

62.14 

77.67 

Z 

X Y 

.000039 


93.21 

x 1.0E+03 

Z 

X Y 

.000119 

Page A.113


Force 

Displacement 

25 

20 

15 

10 

5 

E4 

0 

0 5 10 15 20 25 30 35 40 

E-5 

Time 


4 

2 

0 

-2 

-4 

-6 

-8 

-10 

-12 




Version 7.0 

7-Feb-97 

0 5 10 15 20 25 30 35 40 

E-5 

Time 





Version 7.0 

7-Feb-97 

Page A.114


LS-DYNA Section Manual: *RIGIDWALL_PLANAR 

Example of: Rotating Shell Strikes Stonewall 

Example Filename: rigidwall_shell.key 

Description: 

A rotating shell element strikes and rebounds from a stonewall surface. 

Model: 

The shell element has an elastic material model with Belytschko-Tsay shell formulation. The plate 

measures 10 × 10 × 2 mm 3 . The plate has an initial velocity of 100,000 mm/second in negative zdirection 

and an initial angular velocity of 100,000 radians/second about the y-axis. The rigid 

surface is modeled by an infinite smooth stonewall surface. The termination time is 0.0002 

seconds. 

Input: 

All nodes have initial velocity (*INITIAL_VELOCITY). The location of the “Stonewall” is in the 

x-y plane with z=0 (*RIGIDWALL_PLANAR). The 4 nodes belonging to the shell element are 

slave nodes in the stonewall definition. The velocity components of the slave nodes in the normal 

direction to the stonewall are reset to zero at the moment of impact. 

Reference: 


Page A.115



*KEYWORD 

*TITLE 


$ 

$================================ CONTROL CARDS ================================ 

$ 




$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ] 

2.000E-04 0 .000E+00 .000E+00 .000E+00 





$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 0 0 0 0 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

1.000E-01 .000E+00 1 0 1 0 0 




$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

0 0 0 0 .000E+00 




$ 1 ][ 2 ][ 3 ][ 4 ] 

1 0 1 1 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ][ 8 ] 

0 .000E+00 .000E+00 .000E+00 .000E+00 0 .000E+00 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

0 0 0 0 .000E+00 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 .000E+00 0 .000E+00 .000E+00 0 0 0 


4 1.000E-01 

$ 


$ 


1.000E-05 0 1 



2.000E-03 0 


0 


9999 


1.000E-05 0 


101 


0 0 0 0 0 0 0 0 

0 0 0 

$ 

Page A.116



$ 

*MAT_ELASTIC 

$ Material 1 : ELASTIC MATERIAL 

1 1.000E-08 1.000E+05 .3000 .000E+00 .000E+00 

$ 


$ 


$ Section 1 : ELASTIC MATERIAL 

1 2 .83330 2.0 3.0 .0 0 

1.000E+00 1.000E+00 1.000E+00 1.000E+00 .000E+00 

$ 


$ 

*PART 

ELASTIC MATERIAL 

1 1 1 0 0 0 

$ 

$=================================== NODES ===================================== 

$ 

*NODE 


... 

104 .25000000E+02 .25000000E+02 .10000000E+02 0 0 

$ 

$================================== ELEMENTS =================================== 

$ 



101 2 101 102 104 103 

$ 


$ 

$================================= CONSTRAINTS ================================= 

$ 


$ 

*RIGIDWALL_PLANAR 

1 0 0 


2.000E+01 2.000E+01 .000E+00 2.000E+01 2.000E+01 1.000E+02 .000E+00 


1 

101 102 103 104 

$ 


$ 


101 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 

... 

104 .000E+00 .000E+00-1.000E+05 .000E+00 1.000E+05 .000E+00 

$ 

$================================== LOADING ==================================== 

$ 

*END 

Page A.117


Results: 


Force 

Rigidwall 

10 

8 

6 

4 

2 

Plate 

Initial Position 

Z 

Y 

.000088 

0 

E4 

-2 

0 5 10 15 20 

E-5 

Time 





Version 7.0 

7-Feb-97 

X 

Page A.118


LS-DYNA Manual Section: *INTERFACE_COMPONENT 

Example of: Response of a Cube 

Example File Names: cube_interface_1.key 

cube_interface_2.key 

Execution Line: Initial run: cube_interface_1.key + write interface segment file 

Second run: copy cube_interface_1.isf1 to cube_interface_2.isf2 

cube_interface_2.key + read interface segment file 

Description: 

A cube, one solid element, strikes and rebounds from an elastic plate. In the first run, interface files 

contains the position of the master side of the slideline. In the second run, the cube mesh refinement 

increases from 1 element to 8 elements. The slideline of the first simulation is then tied to the 

slideline of the second simulation. 

Model: 

The material of the cube and the plate are elastic. The plate, that measures 40 × 40 × 2 mm 3 , is 

modeled with 16 Belytschko-Tsay shell elements . The cube has a side length of 10 mm and is 

initially positioned 10 mm above the plate. The initial velocity of the cube is 100 mm/s. The 

calculations will run until 0.0003 seconds. 

Input of the first run: 

The position of the nodes on the surface facing the plate, are recorded every 2 × 10 -6 seconds in the 

Interface-File . The initial velocity of the cube is on the solid element by the Box-Option 

(*INITIAL_VELOCITY). Surface to surface contact, type 3, with thickness projections represents 

the contact between the plate and cube. (*CONTACT_SURFACE_TO_SURFACE, 

*CONTROL_CONTACT) 

Input of the second run: 

The mesh on the cube now contains eight solid elements with new node numbers. The nodes in the 

Interface-File are also defined. Tied surface to surface contact ties the surface to the position of the 

surface in the prior analysis. The prior surface is the master surface and the current surface is the 

slave surface (*INTERFACE_LINKING). 

Reference: 


Page A.119


List of LS-DYNA input deck, first model: 

*KEYWORD 

*TITLE 

INTERFACE SEGMENTS (FIRST ANALYSIS) 

$ 

$================================ CONTROL CARDS ================================ 

$ 




$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ] 

3.000E-04 0 .000E+00 .000E+00 .000E+00 





$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 0 0 0 0 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 .000E+00 0 0 1 0 0 




$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

0 0 0 0 .000E+00 




$ 1 ][ 2 ][ 3 ][ 4 ] 

0 0 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ][ 8 ] 

0 .000E+00 .000E+00 .000E+00 1.000E-01 0 .000E+00 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

0 1000 0 0 2.000E-06 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 1.000E-01 0 .000E+00 .000E+00 0 0 0 


4 .000E+00 

$ 


$ 


1.000E-05 0 1 



5.000E-07 0 


0 


0 


1.000E-05 0 


0 0 0 1 0 0 0 0 

0 0 0 


101 

$ 

Page A.120



$ 

*MAT_ELASTIC 

$ Material 1 : SHELL - STEEL 

1 2.000E-08 1.000E+05 .3000 .000E+00 .000E+00 

$------------------------------------------------------------------------------- 

*MAT_ELASTIC 

$ Material 2 : SHELL -STEEL 

2 1.000E-08 1.000E+05 .3000 .000E+00 .000E+00 

$ 


$ 


$ Section 1 : SHELL - STEEL 

1 0 .83330 2.0 3.0 .0 0 

2.000E+00 2.000E+00 2.000E+00 2.000E+00 .000E+00 

$------------------------------------------------------------------------------- 



2 0 

$ 


$ 

*PART 

SHELL - STEEL 

1 1 1 0 0 0 

$------------------------------------------------------------------------------- 

*PART 

SHELL -STEEL 

2 2 2 0 0 0 

$ 

$=================================== NODES ===================================== 

$ 

*NODE 


1 .00000000E+00 .00000000E+00 .00000000E+00 0 0 

... 

108 .25000000E+02 .25000000E+02 .20000000E+02 0 0 

$ 

$================================== ELEMENTS =================================== 

$ 



101 2 101 102 104 103 105 106 108 107 



1 1 1 2 7 6 

... 

16 1 19 20 25 24 

$ 


$ 



1 1 1 1 1 0 0 0 

... 

25 1 1 1 1 0 0 0 


1 .0 .0 .0 1.0 .0 .0 

.0 1.0 .0 

$ 

$================================= CONSTRAINTS ================================= 

$ 

$ 


$ 

$ 


$ 


0 0 1 

.000E+00 .000E+00-1.000E+05 .000E+00 .000E+00 .000E+00 

*DEFINE_BOX 

1 1.500E+01 2.500E+01 1.500E+01 2.500E+01 1.000E+01 2.000E+01 

$ 

$================================== LOADING ==================================== 

$ 

$ 


$ 


Page A.121


$ NUMBER NAME 

1 Contact # 1 


1 2 0 0 0 0 0 0 


.000E+00 .000E+00 .000E+00 .000E+00 .000E+00 0 .000E+00 .000E+00 


.000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 


0 .000E+00 0 .000E+00 .000E+00 0 0 0 


.000E+00 0 0 

*SET_SEGMENT 

1 .000E+00 .000E+00 .000E+00 .000E+00 

101 103 104 102 .000E+00 .000E+00 .000E+00 .000E+00 

*SET_SEGMENT 

2 .000E+00 .000E+00 .000E+00 .000E+00 

7 8 13 12 .000E+00 .000E+00 .000E+00 .000E+00 

8 9 14 13 .000E+00 .000E+00 .000E+00 .000E+00 

12 13 18 17 .000E+00 .000E+00 .000E+00 .000E+00 

13 14 19 18 .000E+00 .000E+00 .000E+00 .000E+00 

$ 

$================================= INTERFACE =================================== 

$ 

*INTERFACE_COMPONENT_SEGMENT 

$ SET ID 

3 

*SET_SEGMENT 

3 

101 102 104 103 

*END 

Page A.122


List of LS-DYNA input deck, second model: 

*KEYWORD 

*TITLE 

INTERFACE SEGMENTS (SECOND ANALYSIS) 

$ 

$================================ CONTROL CARDS ================================ 

$ 




$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ] 

3.000E-04 0 .000E+00 .000E+00 .000E+00 





$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 0 0 0 0 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 .000E+00 0 0 1 0 0 




$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

0 0 0 0 .000E+00 




$ 1 ][ 2 ][ 3 ][ 4 ] 

0 0 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ][ 8 ] 

0 .000E+00 .000E+00 .000E+00 1.000E-01 0 .000E+00 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

0 1000 0 0 2.000E-06 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 1.000E-01 0 .000E+00 .000E+00 0 0 0 


4 .000E+00 

$ 


$ 


1.000E-05 0 1 



5.000E-07 0 


0 


0 


1.000E-05 0 


201 


0 0 0 1 0 0 0 0 

0 0 0 

$ 

Page A.123



$ 

*MAT_ELASTIC 

$ Material 1 : SHELL -STEEL 

1 1.000E-08 1.000E+05 .3000 .000E+00 .000E+00 

$ 


$ 



1 0 

$ 


$ 

*PART 

SHELL -STEEL 

1 1 1 0 0 0 

$ 

$=================================== NODES ===================================== 

$ 

*NODE 


101 .15000000E+02 .15000000E+02 .10000000E+02 0 0 

... 227 .25000000E+02 .25000000E+02 .20000000E+02 0 0 

$ 

$================================== ELEMENTS =================================== 

$ 



101 1 201 202 205 204 210 211 214 213 

... 108 1 214 215 218 217 223 224 227 226 

$ 


$ 

$ 

$================================= CONSTRAINTS ================================= 

$ 

$ 


$ 

$ 


$ 

$ 

$================================== LOADING ==================================== 

$ 

$ 

$================================= INTERFACE =================================== 

$ 

*INTERFACE_LINKING_SEGMENT 

$ SET ID ifid 

3 1 

*SET_SEGMENT 

3 

201 202 205 204 

202 203 206 205 

204 205 208 207 

205 206 209 208 

*END 

Page A.124


Results of First Model: 

OASYS D3PLOT: INTERFACE SEGMENTS (FIRST ANALYSIS) 

Velocity 

6 

4 

2 

0 

-2 

-4 

-6 

Y 

Z 

X 

.000000000 

-8 

E4 

-10 

0 5 10 15 20 25 30 

E-5 

Time 

Vel z - node 101 

INTERFACE SEGMENTS (FIRST ANALYSIS) 



Version 6.1 

7-Feb-97 

Page A.125


Results of Second Model 

OASYS D3PLOT: INTERFACE SEGMENTS (SECOND ANALYSIS) 

Velocity 

6 

4 

2 

0 

-2 

-4 

-6 

-8 

-10 

E4 

-12 

0 5 10 15 20 25 30 

E-5 

Time 

Vel z - node 201 

INTERFACE SEGMENTS (SECOND ANALYSIS) 



Version 6.1 

7-Feb-97 

Y 

Z 

X 

.000000000 

Page A.126


LS-DYNA Manual Section: *CONTROL_TIMESTEP 

Example of: Billet Upset 

Example Filenames: billet_forge.key 

billet_forge_remap.key 

Execution: Initial run billet_forge.key 

Restart billet_forge_remap.key 

billet_forge_remap.dpf02 

Q = remap 

Description: 

A rod of steel is forged between two dies. The billet upset problem is a measure of friction under 

forming conditions. 

Model: 

The billet material is isotropic elastic-plastic, and the model has 1/8 symmetry. The billet measures 

2.25 inches in height and 1.26 inches in radius. The die compresses the billet 1.60 inches. The 

relationship between the shear friction and the normal pressure is bilinear. 

Input: 

The mass scaling time step size is set to 12 microseconds (*CONTROL_TIMESTEP). The billet 

nodes contact the die surfaces (*CONTACT_NODES_TO_SURFACE). The Coulomb frictional 

constant is 0.10 and the constant shear is 2,055 psi . A half sine wave defines the velocity of the 

die (*DEFINE_LOAD, *BOUNDARY_PRESCRIBED_MOTION). 

Procedure for remapping: 

1. Extract nodal coordinates at the desired time to remap. D3PLOT provides a means for 

dumping nodal coordinates using the 'write' command. 

2. The connectivities of the exterior surface of the original model combined with the deformed 

nodal coordinates define an enclosed discretized surface. 

3. Create a new initial LS-DYNA input deck by remeshing the volume contained by the 

discretized surface. 

4. D3PLOT does not read mixed values of nodes and elements, so move the old binary plot 

files. 

Results: 

The results show that effective plastic strains before and after remapping are unchanged. 

Reference: 

Avitzur, B. Lee, C. H. and Altan, T. 

Page A.127


List of first LS-DYNA input deck: 

*KEYWORD 

*TITLE 

BILLET FORGE 

$ 

$================================ CONTROL CARDS ================================ 

$ 




$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ] 

1.500E-03 0 .000E+00 .000E+00 .000E+00 





$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 0 0 0 0 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 .000E+00 0 0 1 0 0 




$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

0 0 0 0 .000E+00 




$ 1 ][ 2 ][ 3 ][ 4 ] 

0 0 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ][ 8 ] 

0 .000E+00 .000E+00 .000E+00 .000E+00 0 .000E+00 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

0 0 0 0 .000E+00 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 .000E+00 0 .000E+00 1.200E-07 0 0 0 

$ 


$ 


7.333E-06 


7.333E-05 0 1 



2.200E-02 0 


0 


0 


7.333E-05 0 


0 0 0 0 0 0 0 0 

0 0 0 

$ 


$ 

Page A.128



$ Material 1 : BILLET - ALUMINUM 

1 2.500E-04 1.000E+07 .3300 .000E+00 .000E+00 .000E+00 .000E+00 

.000E+00 .000E+00 .0 .0 

.000E+00 5.000E-03 1.000E-02 5.000E-02 1.000E-01 2.000E-01 7.000E-01 4.000E+00 

4.785E+03 6.505E+03 7.423E+03 1.063E+04 1.254E+04 1.482E+04 2.010E+04 3.081E+04 

$------------------------------------------------------------------------------- 

*MAT_RIGID 

$ Material 2 : PRESS - ALUMINUM 

2 2.500E-04 1.000E+07 .3300 .0 .0 .0 

-1.0 .0 110111.0 

.000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 

$ 


$ 


$ Section 1 : BILLET - ALUMINUM 

1 0 

$------------------------------------------------------------------------------- 


$ Section 2 : PRESS - ALUMINUM 

2 0 .00000 .0 .0 .0 0 

1.000E-02 1.000E-02 1.000E-02 1.000E-02 .000E+00 

$ 


$ 

*PART 

BILLET - ALUMINUM 

1 1 1 0 0 0 

$------------------------------------------------------------------------------- 

*PART 

PRESS - ALUMINUM 

2 2 2 0 0 0 

$ 

$=================================== NODES ===================================== 

$ 

*NODE 


1 .00000000E+00 .00000000E+00 .00000000E+00 0 0 

... 

5755 .10646980E+01 .90907520E+00 .11260000E+01 0 0 

$ 

$================================== ELEMENTS =================================== 

$ 



1 1 1 2 11 10 82 83 92 91 

... 

4576 1 5309 5310 3645 3636 5381 5382 3726 3717 



1 2 5383 5394 5395 5384 

... 340 2 5754 5624 5635 5755 

$ 


$ 



1 1 1 1 1 1 1 1 

... 

5319 1 0 1 0 1 0 1 


1 .0 .0 .0 1.0 .0 .0 

.0 1.0 .0 



2 3 0 1 1.000E+00 0 .000E+00 

$ 

$================================= CONSTRAINTS ================================= 

$ 

$ 


$ 

$ 


$ 

$ 


$ 


Page A.129


$ NUMBER NAME 

1 Contact # 1 


1 1 4 0 0 0 1 1 


.100E+00 .100E+00 .000E+00 2.055E+03 .000E+00 0 .000E+00 .000E+00 


.000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 


0 .000E+00 0 .000E+00 .000E+00 0 0 0 


.000E+00 0 0 

$ 


1 

1783 1792 1801 1810 1819 1828 1837 1846 

... 

3077 3158 3239 3320 3401 3482 3563 3644 

*SET_SEGMENT 

1 

5383 5394 5395 5384 

... 

5754 5624 5635 5755 

$ 

$================================== LOADING ==================================== 

$ 

$ 

$=============================== LOAD CURVES =================================== 

$ 

*DEFINE_CURVE 


1 0 .000E+00 .000E+00 .000E+00 .000E+00 

.00000000E+00 .00000000E+00 

... 

.22000000E-02 .00000000E+00 

*END 

Page A.130


List of second LS-DYNA input deck: 

*KEYWORD 

*TITLE 

BILLET FORGE STAGE 2 

$ 

$================================ CONTROL CARDS ================================ 

$ 




$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ] 

2.200E-03 0 .000E+00 .000E+00 .000E+00 





$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 0 0 0 0 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

1.000E-01 .000E+00 0 0 1 0 0 




$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

0 0 0 0 .000E+00 




$ 1 ][ 2 ][ 3 ][ 4 ] 

0 0 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ][ 8 ] 

0 .000E+00 .000E+00 .000E+00 .000E+00 0 .000E+00 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

0 0 0 0 .000E+00 0 0 






$ 1 ][ 2 ][ 3 ][ 4 ][ 5 ][ 6 ][ 7 ] 

.000E+00 .000E+00 0 .000E+00 1.100E-07 0 0 0 

$ 


$ 


7.333E-06 


7.333E-05 0 1 



2.200E-02 0 


0 


0 


7.333E-05 0 


0 0 0 0 0 0 0 0 

0 0 0 

$ 


$ 

Page A.131



$ Material 1 : material type # 24 (elastic-plastic with failure) 

1 2.500E-04 1.000E+07 .3300 .000E+00 .000E+00 .000E+00 .000E+00 

.000E+00 .000E+00 .0 .0 

.000E+00 5.000E-03 1.000E-02 5.000E-02 1.000E-01 2.000E-01 7.000E-01 4.000E+00 

4.785E+03 6.505E+03 7.423E+03 1.063E+04 1.254E+04 1.482E+04 2.010E+04 3.081E+04 

*HOURGLASS 1 4 .000E+00 0 .000E+00 .000E+00 

$------------------------------------------------------------------------------- 

*MAT_RIGID 

$ Material 2 : material type # 20 (rigid body) 

2 2.500E-04 1.000E+07 .3300 .0 .0 .0 

.0 .0 .0 

.000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 

*HOURGLASS 2 4 .000E+00 0 .000E+00 .000E+00 

$ 


$ 


$ Section 1 : material type # 24 (elastic-plastic with failure) 

1 0 

$------------------------------------------------------------------------------- 


$ Section 2 : section properties 

2 0 .00000 .0 .0 .0 0 

1.000E-02 1.000E-02 1.000E-02 1.000E-02 .000E+00 

$ 


$ 

*PART 

material type # 24 (elastic-plastic with failure) 

1 1 1 0 1 0 

$------------------------------------------------------------------------------- 

*PART 

material type # 20 (rigid body) 

2 2 2 0 2 0 

$ 

$=================================== NODES ===================================== 

$ 

*NODE 


1 .00000000E+00 .00000000E+00 .00000000E+00 0 0 

... 5755 .10646982E+01 .90907520E+00 .41185361E+00 0 0 

$ 

$================================== ELEMENTS =================================== 

$ 



1 1 1 2 11 10 82 83 92 91 

... 4576 1 5309 5310 3645 3636 5381 5382 3726 3717 

*ELEMENT_SHELL_THICKNESS 


1 2 5383 5394 5395 5384 

9.99999978E-03 9.99999978E-03 9.99999978E-03 9.99999978E-03 .00000000E+00 

... 340 2 5754 5624 5635 5755 

9.99999978E-03 9.99999978E-03 9.99999978E-03 9.99999978E-03 .00000000E+00 

$ 


$ 



1 1 1 1 1 1 1 1 

... 

5647 1 0 1 0 1 0 1 


1 .0 .0 .0 1.0 .0 .0 

.0 1.0 .0 



2 1 0 2 1.000E+00 0 .000E+00 



2 2 0 2 1.000E+00 0 .000E+00 



2 3 0 1 1.000E+00 0 .000E+00 


Page A.132



2 5 0 2 1.000E+00 0 .000E+00 



2 6 0 2 1.000E+00 0 .000E+00 



2 7 0 2 1.000E+00 0 .000E+00 

$ 

$================================= CONSTRAINTS ================================= 

$ 

$ 


$ 

$ 


$ 

$ 

$================================== LOADING ==================================== 

$ 

$ 


$ 


$ NUMBER NAME 

1* INTERFACE NAME: 1 *** 


1 1 4 0 0 0 0 0 


1.000E-01 1.000E-01 .000E+00 1.502E+03 .000E+00 0 .000E+00 .000E+00 


.000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 .000E+00 


0 .000E+00 0 .000E+00 .000E+00 0 0 0 


.000E+00 0 0 


1 

1783 1792 1801 1810 1819 1828 1837 1846 

... 

3077 3158 3239 3320 3401 3482 3563 3644 

*SET_SEGMENT 

1 .000E+00 .000E+00 .000E+00 .000E+00 

5383 5394 5395 5384 .000E+00 .000E+00 .000E+00 .000E+00 

... 

5754 5624 5635 5755 .000E+00 .000E+00 .000E+00 .000E+00 

$ 

$=============================== LOAD CURVES =================================== 

$ 

*DEFINE_CURVE 


1 0 .000E+00 .000E+00 .000E+00 .000E+00 

.00000000E+00 .00000000E+00 

... 

.22000000E-02 .00000000E+00 

*DEFINE_CURVE 


2 0 .000E+00 .000E+00 .000E+00 .000E+00 

.00000000E+00 .00000000E+00 

.22000000E-02 .00000000E+00 

*END 

Page A.133


Results: 

OASYS D3PLOT: BILLET FORGE 

OASYS D3PLOT: BILLET FORGE 

Y 

Z 

X 

.000000000 


(Mid surface) 

.000 

.252 

.504 

.757 

1.009 

1.261 

1.513 

Y 

Z 

.001500 

X 

Page A.134


OASYS D3PLOT: BILLET FORGE STAGE 2 

OASYS D3PLOT: BILLET FORGE STAGE 2 


(Mid surface) 

.000 

.252 

.504 

.757 

1.009 

1.261 

1.513 

Y 

Z 

.001500 


(Mid surface) 

.000 

.257 

.514 

.771 

1.028 

1.284 

1.541 

Y 

Z 

.002200 

X 

X 

Page A.135


Page A.136


Acknowledgments 

N. Brannberg, L. Fredriksson and A. Gokstorp translated the description of many CADFEM 

examples from German to English. 

References 

Avitzur, B., Handbook of Metal Forming Procedures, John Wiley & Sons, pp. 952-954, 1983 

Belytschko, T., Wong, B. L. and Chiang, H. Y. (Northwestern University) “Improvements in Low- 

Order Shell Elements for Explicit Transient Analysis”, Analytical and Computation Models of 

Shells, Edited by Belytschko, T. and Simo, J., American Society of Mechanical Engineers, 

1989. 

Kenchington, C. J.,“A Non-Linear Elastic Material Model for DYNA3D”, DYNA3D User Group 

Conference, Frazer-Nash Consultancy Ltd., 1988. 

Hallquist, J. O. and Wynn, D. J. “LS-TAURUS: An Interactive Post-Processor for the Analysis 

Codes LS-NIKE3D, LS-DYNA, and TOPAZ3D”, Livermore Software Technology Corporation, 

1992. 

Honecker, A and Mattiasson, K, Finite Element Procedures for 3D Sheet Forming Simulation, 

NUMIFORM 89, pp. 457-464, Balkema, 1989. 

Hughes, T. J. R., The Finite Element Method: Linear Static and Dynamic Finite Element Analysis, 

Stanford University, 1987. 

Lee, C.H., and Altan, T., “Influence of Flow Stress and Friction upon Metal Flow in Upset Forging 

of Rings and Cylinders,” Journal of Engneering for Industry, pp. 775-782, August, 1972. 

Littlewood, T., Correspondence 

Schweizerhof, K. and Weimer, K. CADFEM GmbH, Anzinger Str. 11 D-8017 Ebersberg/Munich, 

Tel 08092 -24012. Correspondence. 

Stillman, D. W., Correspondence. 

Page A.137


Example Input Decks 

Airbag Deploys into Cylinder............................. Page A.3 

Bar Impact ........................................... Page A.62 

Belted Dummy with Springs............................ Page A.100 

Billet Upset ......................................... Page A.127 

Cantilever Beam ...................................... Page A.55 

Cantilever Beam with Lobotto Integration .................. Page A.82 

Corrugated Sheet Contacts Edges......................... Page A.38 

Cube Rebounding from a Rigidwall ...................... Page A.110 

Discrete Nodes Tied to a Surface ......................... Page A.28 

Geometric spherical rigidwall impacts a plate............... Page A.105 

Hemispherical Load ................................... Page A.67 

Hemispherical Punch .................................. Page A.48 

Impulsively Loaded Cap with Shells and Solids ............. Page A.17 

Interaction of Pendulums ............................... Page A.75 

Linearly Constrained Plate .............................. Page A.12 

Piecewise Linear Plasticity Fragmenting Plate ............... Page A.91 

Projectile penetrates Plate ............................... Page A.33 

Rigid Sliding Block in Local Coordinate System ............ Page A.96 

Rigid Sphere impacts Plate .............................. Page A.43 

Rotating Elements ..................................... Page A.87 

Rotating Shell Strikes Stonewall ........................ Page A.115 

Shell Rebounds from Plate Using Five Contact Types ........ Page A.22 

Sliding Blocks with Planar Joint........................... Page A.8 

Twisted Cantilever Beam ............................... Page A.71 

Keywords 

*AIRBAG_SIMPLE_AIRBAG_MODEL ......... Page A.3, Page A.17 

*CONSTRAINED_JOINT_PLANAR ...................... Page A.8 

*CONSTRAINED_LINEAR ............................ Page A.12 

*CONTACT ......................................... Page A.22 

*CONTACT_ENTITY ................................. Page A.43 

*CONTACT_ERODING_SURFACE_TO_SURFACE ....... Page A.33 

*CONTACT_SINGLE_EDGE ........................... Page A.38 

*CONTACT_TIED_NODES_TO_SURFACE .............. Page A.28 

*CONTROL_CONTACT ............................... Page A.48 

*CONTROL_DAMPING ............................... Page A.55 

*CONTROL_ENERGY ................................ Page A.62 

*CONTROL_SHELL ........................ Page A.67, Page A.71 

*CONTROL_TIMESTEP.............................. Page A.127 

*DEFORMABLE_TO_RIGID ........................... Page A.75 

*INTEGRATION_SHELL .............................. Page A.82 

*INTERFACE_COMPONENT ......................... Page A.119 

*LOAD_BODY_GENERALIZED ........................ Page A.87 

Page A.138


*MAT_PIECEWISE_LINEAR_PLASTICITY .............. Page A.91 

*MAT_RIGID........................................ Page A.96 

*MAT_SPRING ..................................... Page A.100 

*RIGIDWALL_GEOMETRIC_SPHERE_MOTION ........ Page A.105 

*RIGIDWALL_PLANAR ............................. Page A.115 

*RIGIDWALL_PLANAR_FORCES ..................... Page A.110 

Page A.139

Oasys LS-DYNA Environment 8.1 VOLUME 3 ... - Oasys Software

You also want an ePaper? Increase the reach of your titles

Delete template?

Save as template?