eta/FEMB-PC TRAINING MANUAL LS-DYNA

eta/FEMB-PC 

(Finite Element Model Builder) 

Version 27 

TRAINING MANUAL 

A pre- and post-processor for use with 

LS-DYNA 

September 2001 

Windows 98/ NT 4/ 2000 

FEMB PC Training Manual Version 27 1

FORWARD 

The concepts, methods, and examples presented in this text are for illustrative and educational 

purposes only, and are not intended to be exhaustive or to apply to any particular engineering problem 

or design. 

This material is a compilation of data and figures from many sources. 

Engineering Technology Associates, Inc. assumes no liability or responsibility to any person or 

company for direct or indirect damages resulting from the use of any information contained herein. 

Engineering Technology Associates, Inc., eta, the eta logo, eta/FEMB-PC, and the eta/FEMB-PC logo 

are the registered trademarks of Engineering Technology Associates, Inc. 

Copyright 2001 Engineering Technology Associates, Inc. All rights reserved. 

Engineering Technology Associates, Inc. 

1133 E. Maple Rd., Suite 200 

Troy, MI 48083-2896 

Phone: (248) 729 - 3010 

FAX: (248) 729 - 3020 

Support: (800) eta – 3362 


FEMB27-PC Tutorial Introduction 

Tutorial-1, Bumper Model 

A half-bumper symmetry model with an initial velocity is crashed against a rigid wall. 

This tutorial presents line mesh and automesh techniques for plate/shell modeling. 

Tutorial-2, LS-DYNA Example Manual pg-55 

Two overlapping plates are connected using spotwelds and the plates are pulled apart. 

This tutorial presents three techniques for plate/shell modeling: 

� Creating Elements by Line Data Meshing 

� Creating Elements by Node Definition 

� Creating Elements By Extrusion 

Most dynamic FEA models require a 5-step setup procedure (pre-process): 

1- Modeling 

2- Material 

3- Property 

4- Contact 

5- BC 

This 5 step procedure will be followed in all the tutorial cases. 


Tutorial-1, Bumper Model 

A symmetrical half-bumper symmetry model with an initial velocity is crashed against a rigid wall. 

This tutorial presents line mesh and automesh techniques for plate/shell modeling. 

STEP-1, Modeling 

Read-in (import) “tutor1.lin” (extension *.lin is FEMB line data file): 

- FILE menu; 

- IMPORT; select “tutor1.lin” file according to your path (in files of type box, select Femb 

Line File, *.lin). 

By default, Lines and Surfaces in the display options are toggled ON. Take the opportunity to switch 

ON/OFF these options to explore the loaded CAD information. Also, use the free rotation, pan and 

zoom commands to explore the line data model. Click the database statistics option to verify the loaded 

entities. Click the part dropdown menu (upper right corner) to verify the number of parts and to 

observe the part color association. 

Four part names will be displayed with their part-color association: 

1- WALL 

2- BUMPER 

3- PLATE 

4- RAIL 


Saving as a FEMB database file (*.fmb): 

- FILE menu; 

- click SAVE AS; input “tutor1” as File Name and *.fmb in the Save As Type box (choose 

the location of the file as desired; the upper left corner of FEMB shows the actual FEMB 

database file name). 


1.1- Creating elements by line data meshing: 

Keep the part Wall on, switch all others off: 

- PART menu (F2); 

- click KEEP; select WALL by clicking on the WALL part name in the data collector; 

APPLY. 

From the part dropdown menu, select WALL to make sure WALL is the current part. The “current 

part” is the active part in which all new entities (i.e., new elements) are created. In FEMB, the “current 

part” is the one showing at the top of the part list dropdown menu. 

Before meshing, we need to know the length of the 4 lines that define the WALL. Using the 

MEASURE/DISTANCE command (ruler icon in the tool bar), measure the lines by clicking on the 

corners, this will show that the wall is 750x500 mm. In this case, we will create 50mm shell elements 

by meshing 15 elements on the long side and 10 on the shorter side the part Wall. 

Element mesh through 4-line mesh: 

- ELEMENT menu (F6); 

- click PLATE/SOLID MESH; 4-LINE; select the 4 lines in the display window by clicking 

on them; 


- insert 15,10 (which is the same as entering 15,10,15,10); 

- click YES to accept the mesh; select END to close the data collector. 

Note: The orientation of line selection dictates the orientation (normal) of the elements to be created 

according to the “right hand rule”. 


1.2- Creating elements by surface data automesh: 

Turn on all the parts but the part Wall: 


- click ON/OFF; turn on all parts but Wall by clicking on the part name; 

- click CLOSE to exit the menu. 

Measure the height of the bumper flange using the measure/distance command (ruler button), ~30.mm. 

Normally, flanges require 2 layers of elements; this would suggest a mesh density (element size) of 

15mm for our sub-system bumper model. 


- click PLATE/SOLID MESH; SURFACE MESH; 

- click BY PART in the data collector; select parts Bumper, Plate, Rail by clicking on the 

part name; APPLY; APPLY; 

- input 15 in the element size popup window; 

- toggle ON “Create elements in original parts” in the popup window (if not, all elements will 

be created in the current part); 

- change Min. internal angle (Quad) to 30; change Max. internal angle (Quad) to 150 (to 

minimize number of tri-elements); 

- click YES to accept the mesh or remesh with a different mesh criteria. 

Turn ON all parts and observe the element mesh result (toggle OFF lines and surfaces, shrink 

elements, rotate model). 


1.3 - Model integrity check: 

After a model is completed, a check for the integrity of the developed model is required. Usually, the 

first check is Boundary Display, which will highlight the free edges of the model and possible 

discontinuities (unconnected elements or other imperfections). 

- CHECK menu (F8); 

- click BOUNDARY DISPLAY; select MULTIPLE SURF. 

Other options can be performed to check the mesh quality (warpage, internal angles, normals, etc). 

Note: The most common discontinuity is when two neighboring elements in a mesh are connected to 

two different nodes sharing the same location or in a small range of proximity instead of connected by 

a single, common node. To fix this imperfection, use the function Check Coincident Node: 

- NODE menu (F5); 

- click CHECK COINCIDENT; 

- input TOLERANCE (range distance of nodes to be merged, i.e., 0.01 default); 

- select the nodes to be verified using the data collector. 


1.4- Connectivity: 

At this point, all parts in the “tutor1.lin” file are modeled and meshed but they are not connected. 

Usually parts are connected by 1-dimensional elements (rigid links or spotwelds). 

Connecting parts by spotwelds: 

First, create a new part called “spotweld”: 


- click CREATE PART; input “spotweld” for new part name; 

- click OK to accept the default values and close the data collector. 

Creating spotwelds: 


- click CREATE; SPOTWELD; 

- switch data collector from POINT to NODE (if not already on NODE); 

- create the spotwelds (two node constraints) by selecting the proper nodes according to the 

following picture: 

� 3 spotwelds on top and bottom of the plate connecting the plate and bumper 

parts 

� 8 spotwelds on each flange of the rail connecting the rail and plate parts 

Note: Turn parts on/off per your convenience when defining the spotwelds. 


STEP-2, Material 

Position the model: 

- turn all parts on; 

- click the ISOMETRIC view button; 

- only ELEMENTS should be toggled on in the Display Options window. 

Note: At this point the CAD information (points, lines, surfaces) has served its purpose and is no 

longer necessary. The information can still remain in the database (toggling lines and surfaces on/off in 

the View Options window), or it can be deleted from the database since a full FEA model has been 

developed from the CAD data. 

1- Material definition: 

- MATERIAL menu (F9) 

Once the material menu is selected FEMB enters the “material mode”. When in material mode the 

graphic window displays parts with material colors instead of part colors. Since no materials have been 

created and assigned yet, our model is displayed in gray. 

In this tutorial, we want to define the part Wall as rigid material and the bumper components (Bumper, 

Plate, Rail) as elasto-plastic material. 

- MATERIAL menu (F9); 

- click CREATE; STRUCTURAL 

- select material 20.1.*MAT_RIGID from the structural material list (a new popup window 

will display for material definition) 

Observe the form/profile of this window and its information: 

a) The left side of the popup window provides the LS-DYNA keyword material name (in this 

case, *MAT_RIGID) and the number of cards required for definition (in this case, 3 cards: 

1.1, 2.1 and 3.1). A check mark is displayed to indicate the active/selected card (in this case, 

1.1). 

b) The adjacent column to the right, Variables, lists the variables for the active/selected card 

(MID, ρ, E, ν, etc.). 

c) The column Description provides a brief description of each variable. 

d) The column Value contains the value defined for each variable. 


Defining parameters: 

- input the following material data (mild steel) on card 1.1: 

ρ, mass density: 7.83E-09 

E, Young’s modulus 2.07E+03 

ν, Poisson’s ratio 0.28 

Note: Rigid material type 20 provides a convenient way of turning one or more parts into a rigid body. 

Approximating a deformable body as rigid is a preferred modeling technique in many real world 

applications. Young’s modulus (E) and Poisson’s ratio (ν) are used for contact friction calculations. 

- select the second card by clicking on card 2.1; 

- input the following parameters: 

CMO 1 (constraints applied in global directions) 

CON1 7 (constrains x,y,z translations) 

CON2 7 (constrains x,y,z rotation) 

- click OK to accept all other default values and close the data collector. 

Defining elasto-plastic material for the bumper components: 


- click CREATE; STRUCTURAL 

- select material 24.1.*MAT_PIECEWISE_LINEAR_PLASTICITY from the structural 

material list; 

- input the following material data in card 1.1: 

ρ, mass density: 7.83E-09 

E, Young’s modulus 2.07E+03 

ν, Poisson’s ratio 0.28 

- select the 3 rd card by clicking on 3.1 and inputting the following plastic strain values to 

define a standard xy stress/strain elasto-plastic curve: 


Effective Plastic Strain 

1- 0.000E+00 

2- 0.309E-01 

3- 0.409E-01 

4- 0.500E-01 

5- 0.151E+00 

6- 0.301E+00 

7- 0.701E+00 

8- 0.910E+00 

- select the 4 rd card by clicking on 4.1 and inputting the following stress values to define a 

standard xy stress/strain elasto-plastic curve: 

Stress Value @EPS# 

1- 0.210E+03 

2- 0.300E+03 

3- 0.314E+03 

4- 0.325E+03 

5- 0.390E+03 

6- 0.438E+03 

7- 0.505E+03 

8- 0.527E+03 


Checking the materials in a database: 


- click LIST. 

The material list is shown according to MID (Material IDentification #) and material name. Two 

materials are currently defined: MID-1 M1 and MID-2 M2. The “stop sign” indicates that the material 

is not currently assigned to any part. 

2- Assigning materials to parts: 


- click ASSIGN; 

- select material M1 (MAT_RIGID) by clicking on it; 

- select part Wall by clicking on it; APPLY. 


- select material M2 (elasto-plastic) by clicking on it; 

- select the parts Bumper, Plate and Rail; APPLY. 

After assigning the materials to the proper parts, the parts assume the material colors while in the 

material menu. 


STEP-3, Properties 





1- Property definition: 

- PROPERTY menu (F10) 

Once the property menu is selected FEMB enters the “property mode”. When in the property mode the 

graphic window displays property colors instead of part colors. Since no properties are created and 

assigned yet, our model is displayed in gray. 

Creating a new property: 

- PROPERTY menu (F10); 

- click CREATE; SHELLS; 

- accept the default values for card 1.1; select the 2 nd card by clicking on 2.1; 

- input 1mm to T1, T2, T3 and T4 (constant 4 node thickness through the shell element); 


For simplicity we will define all parts in this tutorial as 1mm thick. Later on, the user could make this 

analysis more interesting by assigning different thickness/properties to different parts (i.e., Wall=1mm, 

Bumper=1mm, Plate=2mm, Rail=3mm). 

Checking the properties in a database: 


- click LIST. 

The property list is shown according to SECID (SECtion property IDentification #) and property name. 

One property is currently defined: SECID-1 P1. The “stop sign” indicates that the property is not 

currently assigned to any part. 

2- Assigning properties to parts: 



- select property P1 (SECTION_SHELL, 1mm) by clicking on it; 

- select parts Wall, Bumper, Plate and Rail; APPLY. 

After assigning the property to the proper parts, the parts assume the property part color. 


STEP-4, Contact 





1- Contact definition: 

We will define “node to surface” (N2S) contact between the Bumper and the Wall parts: 

- CONTACT menu (F11); 

- click CREATE; 3 DIMENSION; 

*CONTACT_AUTOMATIC_NODES_TO_SURFACE_TITLE; 

- click OK to accept the default name for contact (Contact1) and the Contact ID (1). 

- select the 2 nd card in the DYNA table data collector by clicking on 2.1; 

- click the button in the MSTYP variable value field; select PART ID (MSTYP default value 

of 0 switch to 3, MSTYP=3); 

- click the button in the SSTYP variable value field; select PART ID (SSTYP default value 

of 2 switch to 3, SSTYP=3); 

- click the button in the MSID variable value field and select the part Wall (master contact 

assign to Wall, MSID = PID 1); 

- click the button in the SSID variable value field and select the part Bumper (slave contact 

assign to Bumper, SSID = PID 2); 


After the contact assignment, FEMB displays the defined contact in the Graphic Display Window. 



STEP-5, BC 


- turn all parts on but Wall; 

- click the TOP (xy) view button; 


1- Boundary Condition Definition: 

- BC menu (F12); 

- click BOUNDARY; SPC; CREATE; NODE 

We want to define the symmetry boundary condition for the half bumper mode, which in this case is 

the xy plane (constraint in Y-translation, constraint in X,Z-rotation � SPC=2,4,6). We can define the 

constraint for translation and rotation by toggling on the specific parameters in the popup window or 

by selecting the symmetry plane. 

- toggle on Y-translation and X, Z-rotation, or, click SYMMETRY and select XZ plane; OK; 

- select the nodes in the Bumper part in the symmetry plane (nodes in the lower edge of the 

Bumper as displayed in top view). 



2- Initial Condition Definition: 


- turn all parts on but Wall; 

- click the TOP (xy) view button; 


Defining Initial Conditions: 


- click INITIAL COND; VELOCITY; CREATE; NODE; 

- input Vx= -2234.7 (5 mph); 

- select parts Bumper, Plate and Rail; APPLY; APPLY; 

- CANCEL to finish the command. 


Exporting (outputting) an LS-DYNA Input File: 

All 5 steps are now concluded (modeling, material, property, contact, BC) and we are ready to wrap-up 

for the analyses. The following section describes how to generate the desired output databases for postprocessing. 

The LS-DYNA Miscellaneous drop down menu handles the non-graphical/numerical parameters of 

LS-DYNA (i.e., control termination time, database selection, box definition, etc.). At this point, we 

must define the termination time and output database files. 

Control cards: 

- DYNAMISC menu; 

- click CONTROL; 

- select TERMINATION by clicking into; click DEFINE; 

- input ENDTIM=0.060 sec (60 msec); accept the default for the other variables; 

- click APPLY to accept the data; click OK to close the data collector (TERMINATION flag 

will switch from NO to YES); 

- click CLOSE to exit the Control Window list. 

Database binary: 

- click DATABASE; BINARY; 

- select D3PLOT by clicking on it; click DEFINE; 

- input DT=0.006 sec (6 msec); accept the other default variables; 

- click APPLY to accept the data; click OK to close the data collector (D3PLOT flag will 

switch from NO to YES); 

- click CLOSE to exit the Database Binary window list. 

Database ASCII: 

- click DATABASE; ASCII; 

- select GLSTAT by clicking on it; click DEFINE; 

- input DT=0.0008 sec (0.8 msec); 

- click APPLY to accept the data; click OK to close the data collector (GLSTAT flag will 


- click CLOSE to exit the Database ASCII window list. 

With the above control card definition, we specify the analysis to run 60 msec, the GLSTAT file will 

be written 75 times (60/0.8=75) and the D3PLOT file will be written 10 times (60/0.6=10). The 

number of times that the D3PLOT file is written is equivalent to the number of animation frames in 

post-processing (PostGL). 

We are now ready to write out an LS-DYNA input deck. First, we will check the units: 

- ANALYSIS menu; 

- click SETUP ANALYSIS; 

- in the Analysis Unit dropdown menu select MM, TON, SEC, N; 


- click OK to close the popup window. 

- FILE menu; 

- select EXPORT; 

- input “tutor1” in the File Name box (or other); LS-DYNA File (*.dyn) in the Save As Type 

box;; 

- click SAVE. 

“tutor1.dyn” will be saved and ready for LS-DYNA processing. Take the opportunity to open this file 

in your text editor of choice to get familiar with the LS-DYNA keyword structure. 


Tutorial-2, LS-DYNA Example Manual: *CONSTRAINED_SPOTWELD (pg-55) 

Two overlapping plates are connected using spotwelds and the plates are pulled apart. 

This tutorial presents three techniques for plate/shell modeling: 

� Creating Elements by Line Data Meshing 

� Creating Elements by Node Definition 

� Creating Elements By Extrusion 

Note: Use the FILL and ROTATE command during the tutorial to center the nodes (or other entities) 

in your screen. Also, circumstances may require that the REDRAW command be used. 


STEP-1, Modeling 

1.1- Create a Shell Element Plate 8x4 

Entities (lines, elements, etc.) will always be assigned to a part. Therefore, before creating entities, 

create a part: 


- click create PART; 

- in the popup window input a part name, or accept the default (Part-1); 

- accept the default part parameters in the DYNA Table window by clicking OK (after that, 

you can observe the new part as “current” in the part dropdown list in the upper right corner 

of FEMB). 

OPTION-1 Create Elements by Line Data Meshing 

In this approach, line data is generated or loaded (CAD data). The element mesh is generated on the 

CAD geometry. 

Assuming an empty database with the current part, Part-1: 

1- Line Definition: 

- LINE menu (F3); 

- click CREATE, LINE(S); 

- key-in 0,0,0 and 0,40,0 for the new line coordinates, CREATE, END; 

- LINE menu (F3), COPY, TRANSLATE; 

- select the line by clicking on it, or SELECT ALL in the data collector; 


- click TRANSLATE, GLOBAL; 

- input 80,0,0,1 in the popup window (copy line through x incremental spacing 80, 1 time); 

- answer YES to the “Include copied element in its original part?” popup window prompt; 

- END to close data collector. 

At this point, the two generated lines already define our plate geometry. They allow us to generate 

elements with the 2-line mesh command as follows. The CAD data could be completed if desired and a 

4-line mesh used. 

2- Element Definition: 


- click PLATE/SOLID MESH, 2-LINE MESH; 

- select the 2 lines by clicking on them; 

- input 4,8 (equivalent to 4,8,4,8), accept mesh by clicking YES; 

- END to close the data collector. 

OPTION-2 Create Elements by Node Definition 

In this approach, we generate elements by defining and selecting nodes. Nodes are generated at defined 

coordinates and then copied/translated to define a mesh. 

1- Node Definition: 


- click CREATE, AT COORD (a FEMB data collector window will open for coordinate 

definition); 

- in the data collector window click KEY IN, insert 0,0,0 (tab,tab,enter); 

- click CREATE, END (a node will be created at the origin). 

- in the NODE menu (F5); 

- click COPY, TRANSLATE, (the FEMB data collector window will open for node 

selection and translation input) *; 

- select the node at the origin by clicking directly on the node, or click SELECT ALL (the 

selected node will be highlighted); 


- enter 0,10,0,4 in the popup screen (copy node through y incremental spacing 10, 4 times); 

- click END to close the collector window. 

Another way to define the 5 nodes above: 


- click CREATE, AT COORD; 

- input 0,0,0 and 0,40,0 in the collector window to create 2 nodes at these coordinates; 

- still in the CREATE NODE submenu, select BETWEEN 2 COORD.; 

- switch the data collector from POINT to NODE and click directly on the 2 nodes in the 

graphic display window; 


- enter 3 to generate 3 nodes between the selected nodes; 

- click END to close collector window. 

At this point we have 5 nodes in the y direction spaced by 10. We will copy these 5 nodes along the xy 

plane to generate shell elements with them: 


- click COPY, TRANSLATE; 

- select the 5 nodes BY REGION/DRAG WINDOW from the data collector, or SELECT 

ALL; 


- input 10,0,0,1 in the popup window (copy nodes through x incremental spacing 10, 1 time); 


We now have 10 nodes for element definition. 

Note that the number of nodes and elements can always be verified by observing the lower right edge 

of the FEMB interface. 

2- Element definition: 


- click CREATE, 2D ELEMENT SHELL; 

- select by directly clicking on all 4 adjacent nodes to create 4 shell elements (be sure that the 

data collector is switched to NODE instead of POINT); 


We now have 10 nodes and 4 shell elements. We will copy those elements along the xy plane to define 

a plate mesh: 


- click COPY; 


- click CURRENT PART in the data collector to select all 4 elements (other options to select 

all 4 elements through the data collector are also available), APPLY 

- click MOVE, INCREMENTAL; 

- input 10,0,0,7 in the popup window (copy elements through x incremental spacing 10, 7 

times), GLOBAL; 

- answer YES to the “Include copied element in its original part?” popup window prompt; 

- END to close the data collector. 

We now have 80 nodes and 32 elements defining a plate mesh. 

OPTION-3 Create Elements by Extrusion 

In this approach, the 2-D plate mesh will be generated by the extrusion of 1-D elements. Later, we will 

also use this technique to extrude 3-D solids from 2-D plates. In summary, 1-D elements can be 

extruded to 2-D shell elements, and 2-D shell elements can be extruded to 3-D solid elements. Element 

extrusion is also known as “drag mesh”. 

Assuming an empty database with the current part, Part-1: 

1- Node Definition (5 node definition as before): 


- click CREATE, AT COORD (a FEMB data collector window will open for coordinate 

definition); 

- in the data collector window click KEY IN, insert 0,0,0 (tab,tab,enter); 

- click CREATE, END (a node will be created at the origin). 

- in the NODE menu (F5); 

- click COPY, TRANSLATE, (a FEMB data collector window will open for node selection 

and translation input); 

- select the node at the origin by clicking directly on the node, or click SELECT ALL (the 

selected node will be highlighted); 


- input 0,10,0,4 in the popup screen (copy the node through y incremental spacing 10mm, 4 

times); 


We will generate an extra node for local coordinate definition (for extrusion purposes later); 


- click COPY, TRANSLATE, (a FEMB data collector window will open for node selection 

and translation input); 

- select node 1 (the node at the origin) by clicking on it; 


- input 0,0,10,1 in the popup window (copy the node through z incremental spacing 10mm, 1 

time). 


2- 1D Element Definition: 


- click CREATE, PLOTEL; 

- select the nodes in sequence to generate four 1-D elements (for better viewing, toggle 

SHRINK on in the Display Options Window). 

3- Element Extrusion (1-D to 2-D): 


- click DRAG MESH, TRANSLATIONAL; 

- select the four 1-D elements by clicking on them (or another option from the data collector), 

APPLY; 

- click DEFINE coordinate system; 

- select three nodes for local coordinate system definition by first clicking on the one at the 

origin, then any in the y direction, and then the one in the z direction (the local coordinate 

system will display; the mesh will be generated according to the w local coordinate 

direction); 

- input 80 in the popup window for the drag mesh distance along w axis; 

- input 8 in the popup window for the number of layers along w axis; 

- click YES to accept the mesh. 

The 1-D elements have served their purpose and are no longer necessary. Delete the 1-D elements with 

the DELETE function in the ELEMENT menu (F6). 


1.2- Copy/Translate the Shell Element Plate 

Create a new part: 








- click COPY; 

- select BY PART in the data collector; click on the part name (Part-1) in the data collector 

part list (Part-1 will be selected); APPLY; APPLY; MOVE; INCREMENTAL; 

- input 40,0,2,1 (copy/translate 40mm along x, 2mm along z, 1 time); GLOBAL; 

- answer NO to the “Include copied element in its original part?” popup window prompt; 

- study the model (Free Rotate, Zoom, Fill as necessary) 

1.3- Connecting The Two Plates by Spotweld 

Create a new part: 









- click CREATE; SPOTWELD; 

- click directly on the nodes to generate the spotweld elements as in the following figure 

(make sure that the data collector is toggled on NODE, not POINT); 


The modeling step is done, the next step is to assign material to the parts. 

STEP-2, Material 

- MATERIAL menu (F9) 

Once in material mode the graphic window displays material colors instead of part colors. Since no 

materials are created yet, our model is displayed in gray. 

Defining materials: 

- click CREATE in the material menu; 

- select STRUCTURAL; 

- select material 3.1*MAT_PLASTIC_KINEMATIC; 

- input the following values to the proper material variables: 


Ro = 2.70E-6 

E = 68.9 

Pr = 0.33 

Sigy = 0.286 

Etan = 0.00689 

- click APPLY to accept the data; click OK to close the data collector. 

Material 1 (default name M-1) is created and can be observed by clicking LIST in the material menu. 

Now we’ll assign the material to the proper parts. 

- click ASSIGN in the material menu; 

- select the material (M-1) by clicking directly on the material part list; 

- click ON PARTS in the data collector; APPLY. 

STEP-3, Properties 

- PROPERTY menu (F10) 

Once in the property mode the graphic window displays property colors instead of part colors. Since 

no properties have been created or assigned yet the model is displayed in gray. 

Defining materials: 

- click CREATE in the property menu; 

- select SHELLS; 

- input the following values for these property variables: 

Elform = 6 (S/R Hughes-Liu) 

Nip = 3 

- select the next card by clicking on 2.1 in the left column of the data collector; 

- input the following values for these variables: 

T1 = 2 

T2 = 2 

T3 = 2 

T4 = 2 


Property 1 (default name P-1) is created and can be observed by clicking LIST in the property menu. 

Now we will assign the property. 

- click ASSIGN in the property menu; 

- select the property (P-1) by clicking directly on the property part list; 

- click ON PARTS in the data collector; APPLY. 


STEP-4, Contact 

STEP-5, BC 

- CONTACT menu (F11); 

- click CREATE; select 3 DIMENSION; select 

*CONTACT_AUTOMATIC_SINGLE_SURFACE_TITLE; 

- click OK to accept the default value for Contact Name and Contact ID; 

- click OK to accept the default value (“0”) for all cards (the message window displays: “All 

segments are included for single surface contact”) 

Boundary conditions through SPC definition: 


- click BOUNDARY; SPC; CREATE; select NODE (the data collector will open for SPC 

degree of freedom selection); 

- toggle on X, Y and Z translation (SPC=123); click OK; 

- select all 5 nodes of one side of the lower plate as shown in the following figure; APPLY; 

- toggle on Y and Z translation (SPC=23, X still free); click OK; 

- select all 5 nodes of one side of the upper plate as shown in the following figure; 

- click CANCEL to close the data collector; CLOSE. 


Initial conditions/load by velocity definition on one end of the plate: 

First, we must define a node set: 

- SET menu (F7); 

- click NODE; CREATE; OK to accept the default Set Name and Set ID; 

- select all 5 nodes on the edge of the upper plate previously defined by SPC=23 (not the one 

previously defined by SPC=123); APPLY. 

Then, define a load curve: 


- click LOAD CURVE; CREATE; OK to accept the default load curve name; OK to accept 

the default values for the load curve parameters; 

- input (click INSERT; select KEY-IN) the following XY data for abscissa and ordinate 

curve definition; 

X Y 

0. 0. 

10. 0.3048 

20. 0.3048 

- click OK to close the load curve data collector; CLOSE; 

Prescribed motion definition: 


- click BOUNDARY; PRESCRIBED MOTION; CREATE; NODE SET; 

- in the DYNA Table collector window click on Edit Model button in the NSID value field 

(top right corner of the window) and select Node Set 1 by clicking on it; 

- click on the DOF Enumerated button and select X-TRANSLATION; 

- click on the LCID Edit Model button and select LCur 1 by clicking on it (the above 

variables should look like the following picture); 



All 5 steps are now concluded (modeling, material, property, contact, BC) and we are ready to wrap-up 

for the analyses. The following section describes how to generate the desired output databases for postprocessing. 

Control cards: 


- click CONTROL; 

- select TERMINATION by clicking on it; click DEFINE; 

- input HGEN=8.00; accept the default values for the other variables; 

- click APPLY to accept the data; click OK to close the data collector (TERMINATION flag 

will switch from NO to YES); 

- select ENERGY by clicking on it; click DEFINE; 

- input HGEN=2, SLNTEN=2; accept the default values for the other variables; 

- click APPLY to accept the data; click OK to close the data collector (ENERGY flag will 


- select OUTPUT by clicking on it; click DEFINE; 

- in the NPOPT value dropdown select “NODAL COORDINATES…” (NPOPT=1); in the 

NEECHO value dropdown select “BOTH NODE AND ELEMENT..” (NEECHO=3); 

accept the default values for the other variables; 

- click APPLY to accept the data; click OK to close the data collector (OUTPUT flag will 


- select SHELL by clicking on it; click DEFINE; 

- in the ISTUPID value dropdown select “MEMBRANE…” (ISTUPID=1); accept the default 

values for the other variables; 

- click APPLY to accept the data; click OK to close the data collector (SHELL flag will 


- click CLOSE to exit the Control Window list. 

Database binary: 

- click DATABASE; BINARY; 

- select D3PLOT by clicking on it; click DEFINE; 

- input DT=2; accept the default values for the other variables; 

- click APPLY to accept the data; click OK to close the data collector (D3PLOT flag will 


- select D3THDT by clicking on it; click DEFINE; 

- input DT=99999; accept the default values for the other variables; 

- click APPLY to accept the data; click OK to close the data collector (D3THDT flag will 


- click CLOSE to exit the Database Binary Window list. 

Database ASCII: 

- click DATABASE; ASCII; 

- select GLSTAT by clicking on it; click DEFINE; 

- input DT=0.010; 


- click APPLY to accept the data; click OK to close the data collector (GLSTAT flag will 


- select MATSUM by clicking on it; click DEFINE; 

- input DT=0.010; 

- click APPLY to accept the data; click OK to close the data collector (MATSUM flag will 


- select NODFOR by clicking on it; click DEFINE; 

- input DT=0.010; 

- click APPLY to accept the data; click OK to close the data collector (NODFOR flag will 


- select NODOUT by clicking on it; click DEFINE; 

- input DT=0.010; 

- click APPLY to accept the data; click OK to close the data collector (NODOUT flag will 


- select SECFOR by clicking on it; click DEFINE; 

- input DT=0.010; 

- click APPLY to accept the data; click OK to close the data collector (SECFOR flag will 


- click CLOSE to exit the Database ASCII window list. 

We are now ready to write out an LS-DYNA input deck. First, we will check the units: 

- ANALYSIS menu; 

- click SETUP ANALYSIS; 

- in the Analysis Unit dropdown menu select MM, KG, MSEC, KN; 

- click OK to close the popup window. 

- FILE menu; 

- select EXPORT; 

- input “tutor1” in the File Name box (or other); LSDYNA File (*.dyn) in the Save As Type 

box;; 

- click SAVE. 

“tutor1.dyn” will be saved and is ready for LS-DYNA processing. Take the opportunity to open this 

file in your text editor of choice to get familiar with the LS-DYNA keyword file structure.

eta/FEMB-PC TRAINING MANUAL LS-DYNA

Create successful ePaper yourself

Delete template?

Save as template?