OS-HM-T: 3010 Arthritic Finger, Nonlinear Static Analysis
This tutorial demonstrates nonlinear implicit analysis in OptiStruct involving hyper elastic material and contact.
Figure 1 shows the structural model used for this tutorial: A Hyperelastic Implant connected to bone on both sides. A force of 9 Newtons is applied at one end of the model and the other end of the model is constrained with all degrees of freedom.
The arthritic finger is modeled using hyperelastic material and subjected to a force of 9 N, aiming to rotate the finger by 90 degrees. The results of strain, displacement and stresses are analyzed for the TIE contact.
- Create Hyper Elastic material
- Create Hyper Elastic property
- Set up boundary conditions and imposed load
- Define contact between implant and bones
- Define nonlinear implicit parameters
- Set up NLSTAT analysis
- Submit job and view result
Launch HyperWorks
- Launch Altair HyperWorks.
- In the New Session window, select HyperMesh.
- For Profile, select OptiStruct.
- Click Create New Session.
Import the Model
- On the menu bar, select .
- Navigate to and select Arthritis_Finger.fem.
- Click Open.
- In the Solver Import Options dialog, accept the default settings and click Import.
Set Up the Model
Create Curves
In this step, create the curves for the hyper elastic material.
Define the Hyper Elastic Implant Material
The hyper elastic behavior of the implant must be defined.
- In the Model Browser, right-click and select .
- For Name, enter Implant.
- Click Color and select a color from the color palette.
- For Card Image, select MATHE from the drop-down menu.
- For MODEL, select ABOYCE from the drop-down menu.
- For TAB1, select load-curve TABLES1100.
- For TAB2, select load-curve TABLES1200.
- For TAB4, select load-curve TABLES1400.
- For TABD, select load-curve TABLES1500.
Define the Bone Material
- In the Model Browser, right-click and select .
- For Name, enter Bone.
- Click Color and select a color from the color palette.
- For Card Image, select MAT1 from the drop-down menu.
- For E, enter 14800.
- For NU, enter 0.3.
Define the Implant Property
- In the Model Browser, right-click and select .
- For Name, enter Implant.
- Click Color and select a color from the color palette.
- For Card Image, select PSOLID from the drop-down menu.
- For Material, click .
- In the dialog, select Implant from the list of materials and click OK.
Define the Bone Property
- In the Model Browser, right-click and select .
- For Name, enter Bone.
- Click Color and select a color from the color palette.
- For Card Image, select PSOLID from the drop-down menu.
- For Material, click .
- In the dialog, select Bone from the list of materials and click OK.
Define the Contact Interface Property
- In the Model Browser, right-click and select .
- For Name, enter PCONT.
- Click Color and select a color from the color palette.
- For Card Image, select PCONT from the drop-down menu.
- Under STIFF_REAL_VAL, for STIFF, choose HARD from the drop-down menu.
- Under MU1 Options, for MU1, enter 0.3.
Assign Properties to Components
-
Assign the Implant property.
-
Assign the Bone1 property.
-
Assign the Bone2 property.
Define the Set Segment for the Implant
- In the Component Browser, right-click on Implant and select Isolate from the context menu.
- In the Model Browser, click .
- For Name, enter Implant.
- Click Color and select a color from the color palette.
- For Card Image, select SURF from the drop-down menu.
- For Elements, select .
- In the drop-down menu, select faces.
- Select all faces of the Implant component in the modeling window.
Define the Set Segment for the Bone
Define TIE Contact
- In the Model Browser, right-click and select .
- For Name, enter Tie_Contact.
- Click Color and select a color from the color palette.
- For Card Image, select TIE from the drop-down menu.
- For Secondary Entity IDs, click Implant. and select
- For Main Entity IDs, click Bone. and select
- For DISCRET, select N2S from the drop-down menu.
Apply Loads and Boundary Conditions
Define Nonlinear Implicit Parameters
Define NLADAPT Load Step Inputs
Define NLMON Load Step Inputs
Define NLOUT Load Step Inputs
Define the CNTSTB Load Collector
- In the Model Browser, right-click and select .
- For Name, enter CNTSTB.
- Click Color and select a color from the color palette.
- For Card Image, select CNTSTB from the drop-down menu.
- For S0, enter 0.01.
- For S1, enter 1e-05.
Define the Boundary Condition SPC
Define Force
Define Output Control Parameters
- Select the Analyze ribbon.
- On the drop-down menu for the Run tool group, select Control Cards.
- On the Control Cards panel, select GLOBAL_OUTPUT_REQUEST.
- For all selected output parameters (ELFORCE, SPCF, STRAIN, STRESS), for FORMAT(1), select H3D.
Save the Database
- Click .
- For File Name, enter Arthritis_Finger.hm.
- Click Save.