Super Elastic Alloy Eyeglass Frame Design Using the ANSYS ...

Super Elastic Alloy Eyeglass Frame Design 

Using the ANSYS Workbench Environment 

© 2004 ANSYS, Inc. 

Peter R. Barrett, P.E. 

Patrick Cunningham 

60 Middle Quarter Mall 

Woodbury, CT. 06798 

(203)263-4606 Fax (203)266-9049 

ANSYS, Inc. Proprietary

Analysis Goal 

• The goal of the analysis is to determine the configurations of the 

eyeglass frame that can tolerate being stepped on and still be capable 

of recovery meeting stiffness design requirements. 



Analysis Tools 


• Demonstrate the use of sensitivity analysis at the 

concept stages of an eyeglass frame design. 

• Tools used include: 

– The ANSYS Workbench Environment 

• Parametric geometry is created using DesignModeler 

• Boundary conditions, material constants, and meshing 

controls are defined using the Simulation tool. 

• Sensitivity studies are run using DesignXplorer 

– ANSYS’s super-elastic material model 


Integration of the Analysis Tools 


DesignModeler 

• Develop fully parametric geometry 

models. 

• Remove geometric details that have 

little bearing on the analysis result. 

• Slice up geometry and reform parts 

to enable sweep meshing in the 

Simulation tool. 

DesignXplorer 

• Define tolerances on the input 

• Determine the critical parameters of 

the system. 

• Optimize within the input/response 

characterization. 

• Create a deterministic result of the 

optimum configuration. 

Simulation 

• Define material models. 

• Auto or manually define contact 

element pairs. 

• Apply boundary conditions. 

• Apply Solution Controls. 

• Debug the initial analysis run. 

• Define input and output variables for 

the sensitivity study. 


Design Modeler Parametric Model 

Development 

• The geometric model is built 

using the parametric feature 

capabilities of the 

Workbench/DesignModeler 

tool. 

• Each dimension used in the 

development of the 

geometry is converted to a 

named parameter that is 

accessible as an input 

variable for the sensitivity 

study. 

• Parameter relationships and 

dependences are defined to 

prevent conflicts during 

model regeneration 



Setting up the Analysis Environment 

• Once the geometry is 

complete in DesignModeler it 

is attached in the Simulation 

Tool 

• Meshing, material properties, 

boundary conditions, and 

solution controls are defined 

in the solution tool 

• Toggling between the design 

and analysis tools is possible 

at any time using the 

Workbench tabs 



Meshing in Workbench 

• DesignModeler is also 

used to slice the 

geometry in the 

desired regions to 

enable automatic 

sweep meshing in the 

DesignSimulation 

tool. 

• Mesh sizing controls 

are added in the 

DesignSimulation 

tool. 

• A coarse finite 

element mesh is used 

for this example. 



Super Elastic Material Model 

• Nitinol is an acronym for Nickel Titanium Naval 

Ordinance Laboratory since the alloy was 

originally developed at the U.S. Naval Laboratory. 

• It is used to describe a family of materials, which 

contain a nearly equal mixture of nickel and 

titanium. 

• Nitinol alloys are attractive because they are 

biocompatible and are at their optimum superelastic 

behavior (9% strain fully recoverable) at 

room temperature when processed properly. 



Stress vs. Strain for a Nitinol Material 

Model using ANSYS 


• Constant Definition 

• SIG-SAS (C1) Starting stress value for the forward phase transformation 

• SIG-FAS (C2) Final stress value for the forward phase transformation 

• SIG-SSA (C3) Starting stress value for the reverse phase transformation 

• SIG-FSA (C4) Final stress value for the reverse phase transformation 

• EPSILON (C5) Maximum residual strain 

• ALPHA (C6) α material responses ratio between tension and compression 

• YMRT (C7) Modulus for Martensite (This is Beta in 8.0/8.1) 


Material properties 

• The material 

properties are 

defined in the 

Simulation tool 

using the 

Preprocessing 

Command Builder. 

• The Preprocessing 

Command Builder 

enables access to 

the ANSYS 

material model 

GUI. 



Creating Rigid Target Surfaces 

• In the Workbench Simulation 

module contact pairs are 

automatically defined between 

adjacent parts when the 

geometry is attached. 

• For this case we have opted 

to define the crushing 

surfaces as rigid target 

elements which do not require 

underlying solid elements. 

• As a result, the rigid target 

surfaces and the contact pairs 

are defined using APDL 

commands. 



Creating contact pairs using APDL 

• The first step in the APDL 

generation of the contact 

pairs is to identify the 

surfaces on the model 

where the contact elements 

will be generated. 

• This is easily done by 

defining Named Selections 

for the top and bottom 

surfaces in the Simulation 

tool. 



Named Components in Workbench 

• The named surface 

selections on the solid 

geometry will be 

transferred to ANSYS 

as nodal components. 

• Named Solids will be 

transferred as Element 

Groups 

• Loads are transferred 

as surface effect 

elements that can be 

further modified in 

ANSYS 



Defining Contact Pairs using APDL 


Commands worksheet is 

used to define the target 

elements in the following 

fashion: 

– Use *get commands to 

determine the maximum 

element type number and 

real table defined. 

– Define new contact and 

target element type 

numbers. 

– Define new real tables for 

the contact pairs 

– Use APDL commands to 

directly generate the nodes 

and elements of the rigid 

target surfaces. 





Commands worksheet 

is also used to define 

the contact elements: 


– Select the nodal 

components of the top 

and bottom surfaces. 

– Select solid elements 

attached to the nodes. 

– Specify element 

attributes. 

– Use ESURF to generate 

the contact elements. 




Notes: 

– A self contact pair is defined around the perimeter of 

the lens frame. This pair could also have been defined 

using the manual contact capability in the Workbench 

Simulation tool. 

– The target surfaces could also be defined using 

surface geometry and the resulting shell elements 

converted to rigid target elements using the EMODIF 

command in the Preprocessing Commands worksheet. 


Boundary Conditions 

• The following boundary conditions 

are applied to the model: 

1. A frictionless support is applied 

on the bridge of the glasses to 

establish reflective symmetry. 

This is applied as a support 

inside the Simulation 

environment. 

2. The lower rigid target is fixed in 

all degrees of freedom. This 

constraint is defined using the 

Processing Command 

worksheet. 

3. The upper rigid target is 

displaced –1” in the vertical 

direction. This constraint is 

defined using the Processing 

Command worksheet. 



Solution Controls 

• The nonlinear solution 

controls are defined 

using the Preprocessing 


• Multiple load steps 

(loading and unloading) 

are defined using the 

solution controls menu. 

• Does require adding 

SOLVE commands to the 

Preprocessor Command 

Builder 



Initial Solution in the Simulation Tool 

• Prior to the sensitivity 

study, an initial solution 

is generated by solving 

in the Simulation 

environment. 

• This is not a required 

step, but it is always 

recommended, 

particularly for debugging 

the nonlinear solution. 



Postprocessing the initial Simulation 

• Postprocessing of the 

initial simulation run can 

be done with a 

combination of the 

standard Simulation 

solution tools and the 

Postprocessing 


• The Simulation 

environment only has 

access to the last 

converged solution and 

the results are limited to 

linear quantities with the 

exception on contact 

results. 



Postprocessing the initial simulation 

• The Postprocessing 

Command builder can be 

used to look at the full 

contents of the ANSYS 

result file. 

• All results steps written 

to the ANSYS result file 

are accessible. 

• All nonlinear results are 

accessible 

• Time history plots and 

result combinations are 

also possible using the 

result viewer. 



Time History plots using the Postprocessing 


• The Postprocessing Command builder can be used to plot the 

hysteresis response of the shape memory alloy. 



Time History plots using the Postprocessing 


• Result plots and 

listings from the 

Postprocessing 


can be returned to 

the Simulation 

Environment. 

These figures are 

then included in the 

design report. 



Setting up the Sensitivity study environment 

• Once the initial solution is 

resolved, input and output 

variables for the sensitivity 

study are defined in the 

simulation environment. 

• Input and output variables are 

defined by checking the box to 

the left of the parameter. 

• In this case we specify the 

defining geometric parameters 

as the input variables 



Setting up the Sensitivity study environment 

• The output variables 

for this study are the 

Von Mises stress and 

the deformation in the 

load direction. 

• The stress can be used 

to simulate the elastic 

response, while the 

displacement is used 

to measure stiffness 



DOE Method of Design Explorer 

• When the data is 

attached to a 

DesignXplorer 

session, the upper 

and lower bounds 

(or discrete values) 

of the input variables 

must be defined. 



Design Explorer DOE – Solution 

• For the DOE method 

used by 

DesignXplorer the 

number of 

deterministic 

solutions required is 

automatically 

determined based 

on the number of 

input variables. 




• Sensitivity of Max. 

Von Mises stress vs. 

Frame thickness and 

Frame bottom radius 

are illustrated in the 

Figure. 

• As expected the larger 

the larger radius / 

thinner frame 

produces the lowest 

stress values 

• Specific data is 

extracted from the 

Response Tabs 




• “Soft” Design Sets 

are created in 

Design Explorer 

directly from the 

DOE 

• A chosen design can 

then be run explicitly 

to get the hard 

design results 

• Data can also be 

exported to a 

spreadsheet for 

integration into 

design rules, etc. 



Conclusions 

• The combination of design modeler, 

design simulation and design 

explorer provide a valuable tool for 

upfront engineering 

• Complex material models and 

Highly nonlinear analyses were 

easily adapted into the workbench 

environment 

• Sensitivity results (example on 

right) provide valuable data for the 

design engineer to quickly 

determine the most relevant design 

parameters

Super Elastic Alloy Eyeglass Frame Design Using the ANSYS ...

Create successful ePaper yourself

Delete template?

Save as template?