OS-HWX-T: 3010 Arthritic Finger, Nonlinear Static Analysis

This tutorial demonstrates nonlinear implicit analysis in OptiStruct involving hyper elastic material and contact.

Before you begin, copy the file(s) used in this tutorial to your working directory.


Figure 1. Model and Loading Description

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.

The following exercises are included:
  • 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

  1. Launch HyperWorks.
  2. In New Session, under HyperWorks select HyperMesh.
  3. For Profile, select OptiStruct.
  4. Click Create New Session.

Import the Model

  1. On the menu bar, select File > Import > Solver Deck.
  2. Navigate to and select Arthritis_Finger.fem.
  3. Click Open.
  4. 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.

  1. In the Model Browser, right-click and select Create > Curve.
    A default window for the Curve Editor opens.
  2. Right-click on the new table and select Rename.
  3. For name, enter TABLES1100.
  4. Enter the following values in the X and Y fields:
    Table 1. Simple Tension Compression Data Values
    X (stress) Y (strain)
    1.1338 1.5506
    1.2675 2.4367
    1.3567 3.1013
    1.6242 4.2089
    1.8917 5.3165
    2.1592 5.981
    2.4268 6.8671
    3.051 8.8608
    3.586 10.6329
    4.0318 12.4051
    4.7898 16.1709
    5.3694 19.9367
    5.8153 23.481
    6.172 27.4684
    6.4395 31.0127
    6.707 34.557
    6.9299 38.3228
    7.0637 42.0886
    7.1975 45.6329
    7.3312 49.3987
    7.465 53.1646
    7.5541 56.9304
    7.6433 64.2405


    Figure 2.
  5. Click Close.
  6. In the Model Browser, double-click Curves and select TABLES1100.
  7. For Card Image, select TABLES1 from the drop-down menu.
  8. Create another curve for equi-biaxial tension.
    1. For Name, enter TABLES1200.
    2. Enter the following values in the X and Y fields:
      Table 2. Equi-biaxial Tension Data Values
      X Y
      1.02 0.9384
      1.06 1.59
      1.11 2.4087
      1.14 2.622
      1.2 3.324
      1.31 4.4278
      1.42 5.183
      1.68 6.6024
      1.94 7.7794
      2.49 9.7857
      3.03 12.6351
      3.43 14.6804
      3.75 17.4
      4.07 20.1058
      4.26 22.4502
      4.45 24.653
    3. For Card Image, select TABLES1.
  9. Create another curve for pure shear loading data.
    1. For Name, enter TABLES1400.
    2. Enter the following values in the X and Y fields:
      Table 3. Pure Shear Loading Data Values
      X Y
      1.069 0.6
      1.1034 1.6
      1.1724 2.4
      1.2828 3.36
      1.4276 4.2
      1.8483 6
      2.3862 7.8
      3.0 9.6
      3.4897 11.12
      4.0345 12.96
      4.4483 14.88
      4.7793 16.58
      5.0621 18.2
    3. For Card Image, select TABLES1.
  10. Create another curve for volumetric data.
    1. For Name, enter TABLES1500.
    2. Enter the following values in the X and Y fields:
      Table 4. Volumetric Data Values
      X Y
      0.9703 60
      0.9412 118.2
      0.9127 175.2
      0.8847 231.1
    3. For Card Image, select TABLES1.

Define the Hyper Elastic Implant Material

The hyper elastic behavior of the implant must be defined.

  1. In the Model Browser, right-click and select Create > Material.
  2. For Name, enter Implant.
  3. Click Color and select a color from the color palette.
  4. For Card Image, select MATHE from the drop-down menu.
  5. For MODEL, select ABOYCE from the drop-down menu.
  6. For TAB1, select load-curve TABLES1100.
  7. For TAB2, select load-curve TABLES1200.
  8. For TAB4, select load-curve TABLES1400.
  9. For TABD, select load-curve TABLES1500.

Define the Bone Material

  1. In the Model Browser, right-click and select Create > Material.
  2. For Name, enter Bone.
  3. Click Color and select a color from the color palette.
  4. For Card Image, select MAT1 from the drop-down menu.
  5. For E, enter 14800.
  6. For NU, enter 0.3.

Define the Implant Property

  1. In the Model Browser, right-click and select Create > Property.
  2. For Name, enter Implant.
  3. Click Color and select a color from the color palette.
  4. For Card Image, select PSOLID from the drop-down menu.
  5. For Material, click Unspecified > Material.
  6. In the dialog, select Implant from the list of materials and click OK.

Define the Bone Property

  1. In the Model Browser, right-click and select Create > Property.
  2. For Name, enter Bone.
  3. Click Color and select a color from the color palette.
  4. For Card Image, select PSOLID from the drop-down menu.
  5. For Material, click Unspecified > Material.
  6. In the dialog, select Bone from the list of materials and click OK.

Define the Contact Interface Property

  1. In the Model Browser, right-click and select Create > Property.
  2. For Name, enter PCONT.
  3. Click Color and select a color from the color palette.
  4. For Card Image, select PCONT from the drop-down menu.
  5. Under STIFF_REAL_VAL, for STIFF, choose HARD from the drop-down menu.
  6. Under MU1 Options, for MU1, enter 0.3.

Assign Properties to Components

  1. Assign the Implant property.
    1. In the Component Browser, select Implant.
    2. For Property, click Unspecified > Property and select Implant from the list.
      The Material field is auto-filled with Implant.
    3. Click OK.
  2. Assign the Bone1 property.
    1. In the Component Browser, select Bone1.
    2. For Property, click Unspecified > Property and select Bone from the list.
      The Material field is auto-filled with Bone.
    3. Click OK.
  3. Assign the Bone2 property.
    1. In the Component Browser, select Bone2.
    2. For Property, click Unspecified > Property and select Bone from the list.
      The Material field is auto-filled with Bone.
    3. Click OK.

Define the Set Segment for the Implant

  1. In the Component Browser, right-click on Implant and select Isolate from the context menu.
  2. In the Model Browser, click Create > Set Segment.
  3. For Name, enter Implant.
  4. Click Color and select a color from the color palette.
  5. For Card Image, select SURF from the drop-down menu.
  6. For Elements, select 0 Elements > Elements.
  7. In the drop-down menu, select faces.
  8. Select all faces of the Implant component in the modeling window.

Define the Set Segment for the Bone

  1. In the Component Browser, right-click on Bone1 and Bone2 and select Isolate from the context menu.
  2. In the Model Browser, click Create > Set Segment.
  3. For Name, enter Bone.
  4. Click Color and select a color from the color palette.
  5. For Card Image, select SURF from the drop-down menu.
  6. For Elements, select 0 Elements > Elements.
  7. In the drop-down menu, select faces.
  8. Select all inside faces of the Bone1 and Bone2 components in the modeling window.


    Figure 3.


    Figure 4.

Define TIE Contact

  1. In the Model Browser, right-click and select Create > Contact.
  2. For Name, enter Tie_Contact.
  3. Click Color and select a color from the color palette.
  4. For Card Image, select TIE from the drop-down menu.
  5. For Secondary Entity IDs, click Unspecified > Set Segment and select Implant.
  6. For Main Entity IDs, click Unspecified > Set Segment and select Bone.
  7. For DISCRET, select N2S from the drop-down menu.

Apply Loads and Boundary Conditions

Define Nonlinear Implicit Parameters

  1. In the Model Browser, right-click and select Create > Load Step Inputs.
    A default load step input editor window opens.
  2. For Name, enter NLPARM.
  3. For Config Type, select Nonlinear Parameters from the drop-down menu.
    By default, for Type NLPARM is selected.

Define NLADAPT Load Step Inputs

  1. In the Model Browser, right-click and select Create > Load Step Inputs.
    A default load step input editor window opens.
  2. For Name, enter NLADAPT.
  3. For Config Type, select Time step Parameters from the drop-down menu.
    By default, for Type NLADAPT is selected.
  4. Select the NCUTS check box and enter a value of 25 in the text box.

Define NLMON Load Step Inputs

  1. In the Model Browser, right-click and select Create > Load Step Inputs.
    A default load step input editor window opens.
  2. For Name, enter NLMON.
  3. For Config Type, select Runtime Monitoring from the drop-down menu.
    By default, for Type NLMON is selected.
  4. For ITEM, select DISP from the drop-down menu.
  5. For INT, select ITER from the drop-down menu.

Define NLOUT Load Step Inputs

  1. In the Model Browser, right-click and select Create > Load Step Inputs.
    A default load step input editor window opens.
  2. For Name, enter NLOUT.
  3. For Config Type, select Output Parameters from the drop-down menu.
    By default, for Type NLOUT is selected.
  4. For Nonlinear Incremental Output, select NINT from the drop-down menu.
  5. For VALUE, enter 10.
  6. Select the SVNONCNV check box and for VALUE, select YES.

Define the CNTSTB Load Collector

  1. In the Model Browser, right-click and select Create > Load Collector.
  2. For Name, enter CNTSTB.
  3. Click Color and select a color from the color palette.
  4. For Card Image, select CNTSTB from the drop-down menu.
  5. For S0, enter 0.01.
  6. For S1, enter 1e-05.

Define the Boundary Condition SPC

  1. In the Model Browser, right-click and select Create > Load Collector.
  2. For Name, enter spc.
  3. Click Color and select a color from the color palette.
  4. Open the Analyze ribbon and select BCs > Constraints.
    A panel to define the constraint opens.
  5. On the first drop-down menu in the panel, select nodes.
  6. On the second drop-down menu, select faces.
  7. In the modeling window, select the entire rear side face (all nodes) of Bone1.
  8. For load types, select SPC.
  9. Select all dof check boxes and enter 0.0 in the corresponding text boxes.


    Figure 5.


    Figure 6.

Define Force

  1. In the Model Browser, right-click and select Create > Component.
  2. For Name, enter RBE2.
  3. Click Color and select a color from the color palette.
  4. On the guide bar, select Dependent and choose faces from the drop-down menu.
  5. Select the front face of Bone2 and click .


  6. In the Model Browser, click Create > Load Collector.
  7. For Name, enter Force.
  8. Click Color and select a color from the color palette.
  9. Select the Analyze ribbon.
  10. On the Loads tool, select the Forces sub tool.


    Figure 7.
    The corresponding panel opens.
  11. In the modeling window, select the center node of RBE2.
  12. For magnitude, enter 9.0.
  13. From the drop-down menu below magnitude, select x-axis.
  14. For load types, select FORCE.


Define Output Control Parameters

  1. Select the Analyze ribbon.
  2. On the drop-down menu for the Run tool group, select Control Cards.
  3. On the Control Cards panel, select GLOBAL_OUTPUT_REQUEST.
  4. For all selected output parameters (ELFORCE, SPCF, STRAIN, STRESS), for FORMAT(1), select H3D.

Save the Database

  1. Click File > Save.
  2. For File Name, enter Arthritis_Finger.hm.
  3. Click Save.

Run the Analysis

  1. Select the Analyze ribbon.
  2. In the Run tool group, select Run OptiStruct Solver.
  3. Click save as.
  4. In the Save As dialog, specify location to write the OptiStruct model file and enter Arthritis_Finger for filename.
    For OptiStruct input decks, .fem is the recommended extension.
  5. Click Save.
    The input file field displays the filename and location specified in the Save As dialog.
  6. Set the export options toggle to all.
  7. Set the run options toggle to analysis.
  8. Set the memory options toggle to memory default.
  9. Click OptiStruct to run the analysis.
    If the job was successful, new files are available in the directory where you chose to write the files. OptiStruct also reports error messages if any exist. The file Arthritis_Finger.out can be opened in a text editor to find details regarding any errors. This file is written to the same directory as the .fem file.

View the Results

  1. In the Solver window, select Results to open the results in HyperView.
  2. HyperView, select Contour .
  3. For Results Type, in the first drop-down menu, select Element Stresses (2D & 3D) (t).
  4. For Results Type, in the second drop-down menu, select vonMises.


    Figure 8. Contour of Element Stresses in Bone and Implant Subject to Loading


    Figure 9. Contour of Displacement in Bone and Implant Subject to Loading


    Figure 10. Contour of Element Strains in Bone and Implant Subject to Loading