OS-T: 1393 Basics of Contact Properties and Debugging

This tutorial demonstrates the effect of using contact stabilization, clearance, adjust and smoothing.

The model consists of two circular parts where the inner one is heated and the outer one cooled down, leading to contact between the two. The effect of using several important contact settings such as contact stabilization, clearance, adjust and smoothing on both the results and the convergence behavior is considered.

The model consists of two circular parts where the inner one is heated and the outer one cooled down, leading to contact between the two. The effect of using several important contact settings such as contact stabilization, clearance, adjust and smoothing on both the results and the convergence behavior is considered.

os_1393_model
Figure 1. Illustration of the Model

Launch HyperMesh and Set the OptiStruct User Profile

  1. Launch HyperMesh.
    The User Profile dialog opens.
  2. Select OptiStruct and click OK.
    This loads the user profile. It includes the appropriate template, macro menu, and import reader, paring down the functionality of HyperMesh to what is relevant for generating models for OptiStruct.

Import the Model

  1. Click File > Import > Solver Deck.
    An Import tab is added to your tab menu.
  2. For the File type, select OptiStruct.
  3. Select the Files icon files_panel.
    A Select OptiStruct file browser opens.
  4. Select the wheels_contact.fem file you saved to your working directory from the optistruct.zip file. Refer to Access the Model Files.
  5. Click Open.
  6. Click Import, then click Close to close the Import tab.

    The outline of the Fatigue Analysis setup to be achieved in the following steps.

Set Up the Model

Create a PCONT Property

The imported model already contains the material, the property, the boundary conditions and the loadstep, the contact surfaces and the Contact. In this step, a PCONT property is created.
  1. In the Model Browser, right-click and select Expand All.
  2. Right-click in the Model Browser, and select Create > Property to create a PCONT property.
  3. For Name, enter cont_prop.
  4. Open the Entity Editor by selecting the newly created property in the Model Browser.
  5. In the Entity Editor, change the Card Image to PCONT.

    os_1393_pcont
    Figure 2. Changing the PCONT Contact Property
  6. In the Model Browser, select the interface cont_interf to assign the property to the interface.
  7. In the Entity Editor, select Property Id as the property and change the PID to cont_prop.

Submit the Job

  1. From the Analysis page, enter the OptiStruct panel.

    OS_1000_13_17
    Figure 3. Accessing the OptiStruct Panel
  2. Click save as following the input file field.
    The Save As dialog opens.
  3. Select the directory where you would like to write the OptiStruct model file and enter the name for the model, Contact_S2S.fem, in the File name field.
    For OptiStruct input decks, .fem is the recommended extension.
  4. Click Save.
    The name and location of the Contact_S2S.fem file displays in the input file field.
  5. Set the export options toggle to all.
  6. Set the run options toggle to analysis.
  7. Set the memory options toggle to memory default.
  8. Click OptiStruct. This launches the OptiStruct job.
    If the job is successful, the new results files should be in the directory from which Contact.fem was selected. The Contact_S2S.out file is a good place to look for error messages that could help debug the input deck if any errors are present.

Add Contact Stabilization

Since the non-linearity of this model is only due to contact, a good way to overcome the convergence issues is to add contact stabilization. This will especially be useful when part of the structure is held in place by the contact, which is the case here.
  1. Click Setup > Create > Control Cards.
  2. Select PARAM and check the box next to EXPERTNL.
  3. Select CNTSTB.
    Also, contact stabilization can be activated through the Bulk Data card CNTSTB and referencing it from within the subcase. This gives you more options.
  4. Repeat Submit the Job, with the new file name Contact_CNTSTB.fem.

    os_1393_param_exprtnl
    Figure 4. Creating PARAM,EXPERTNL,CNTSTB

Add Clearance

Now you want to investigate the influence of clearance on the model.
  1. In the Model Browser, select the cont_prop property.
  2. In the Entity Editor, click on the field next to CLEARANCE and enter the value 0.1.
    Clearance will internally set the gap between the surfaces to the real value chosen, independently of the actual position of the grids, if grids are not moved to achieve this.

    os_1393_cont_prop
    Figure 5. Change the PCONT Contact Property
  3. Repeat Submit the Job, with the new file name Contact_Clearance.fem.

Add AUTO Adjust

Now you want to investigate the influence of adjust on the model. First, remove the clearance you defined in Add Clearance.
  1. In the Model Browser, select the property cont_prop.
  2. In the Entity Editor, click on the field next to CLEARANCE and remove the previously inserted value of 0.1.
  3. In the Model Browser, select the interface cont_interf.
  4. In the Entity Editor, click on the field next to ADJUST and select AUTO.

    os_1393_cont_interf
    Figure 6. Change the Parameters of the CONTACT
  5. Repeat Add Clearance, with renaming the file Contact_Adjust.fem.

Apply Surface Smoothing

  1. In the Model Browser, select the interface cont_interf.
  2. In the Entity Editor, click on the field next to ADJUST and set to blank.
  3. For CONTACT_NUM_SMOOTH, enter 1.
  4. Click on the field next to SMSIDE and select BOTH and ALL.

    os_1393_contact_surf_smooth
    Figure 7. Select the Surface Smoothing Option on the CONTACT Card
  5. Repeat Submit the Job, with the file name Contact_Smoothing.fem.

View the Results

Displacements, Element Stresses, Contact Force, Contact Deformation, Contact Status and Contact Traction are calculated and can be plotted using the Contour panel in HyperView. Only compare the Contact Traction between the N2S and the S2S run.

Compare the Contact Traction

  1. Launch HyperView.
  2. Select the page window layout icon pageLayout4-24 to split the page into four windows.
  3. Click fileImportModel-24 to load the first model in one of the window.
  4. Select Contact_CNTSTB.h3d for model and results.
  5. Click Apply.
  6. Do the same in the other three windows for Contact_Clearance.h3d, Contact_Adjust.h3d and Contact_Smoothing.h3d.
  7. Click the Contour toolbar icon resultsContour-16 in one of the four windows.
  8. For Result type, select Contact Traction/Normal(s).
  9. Click Apply.

    os_1392_contour_plot
    Figure 8. Contour Plot Panel in HyperView
  10. In the Entity Editor, unselect the outer part of the structure.
    Only the results on the contact surface will be visible.
  11. Right-click in the window that shows the contour and select Apply Style > Current Page > All selected to view the same results for both models.
  12. A contour plot of normal contact traction shows for both runs.
    The traction for the runs with clearance and adjust are more uniform than they are for the model with stabilization only. The surface smoothing leads to a more uniform contour. In addition, the peaks are much lower for these three models. The reason why is, the traction is much higher for adjust than it is for the clearance, and the adjust run is that for adjust, the gap is closed initially, which leaves less room for stress free thermal expansion as for the other runs.

    os_1392_apply_style_menu
    Figure 9. Apply the Setup in One Window to the Rest of the Page

    os_1393_contact_traction
    Figure 10. Normal Contact Traction Contour for the Four Different Runs