OS-T: 1392 Node-to-Surface versus Surface-to-Surface Contact

This tutorial demonstrates how to set up contact between two parts and the impact of using choosing node-to-surface (N2S) versus surface-to-surface (S2S). In addition, this tutorial covers how to review the internally created CGAPG elements in case of N2S, and the nodes in contact in case of S2S.

Before you begin, copy the file(s) used in this tutorial to your working directory.
The model consists of two cubes in contact and enforced displacement on the top compressing the structure.

os_1392_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 blocks_contact.fem file you saved to your working directory.
  5. Click Open.
  6. Click Import, then click Close to close the Import tab.

Set Up the Model

Create Set Segments

The imported model already contains the material, the property, the boundary conditions and the loadstep. In this step, the set segments and the interface are created.
  1. In the Model Browser, right-click and select Expand All.
  2. Right-click in the Model Browser and select Create > Set Segment to create a set segment.

    os_1392_contact_surface_menu
    Figure 2. Create a Set Segment from the Model Browser
  3. For Name, enter bottom.
  4. In the Model Browser, right-click on the component bottom under Component and select Isolate Only.
  5. To add elements and their faces to the surface, select the bottom set segment in the Model Browser and click on 0 Elements in the Entity State Browser.
  6. Click Element to select elements from the panel. Switch the selector to Solid faces, as this contact surface will be on solid elements.
  7. Switch the second drop-down menu to elems.
  8. Click elements and click displayed to select all elements from the bottom part of the structure.
  9. Select three nodes on the surface that are in contact with the top part. Make sure the three nodes are all part of one element.
  10. Click return to finish.
  11. Repeat steps 3 through 9 to create the top part.

    os_1392_add_contact_surface
    Figure 3. Add a Set Segment

Create the Contact Interface

After defining the two contact surfaces using set segments, you need to define that they are in contact and with which properties. A contact interface needs to be defined.
  1. In the Model Browser, right-click and select Create > Contact.
  2. For Name, enter top_to_bottom.
  3. In the Model Browser, select the newly created Contact to modify the properties of the contact.
  4. For TYPE, select SLIDE.
    This will result in a frictionless contact.
  5. To select the secondary surface, click on the field next to Secondary Entity IDs.
    The secondary surface should be the finer side, in this case the bottom (refer to the User Guide).
  6. Select the top for Main Entity IDs.
  7. For DISCRET, select N2S.
  8. Retain the default values in the remaining fields, for now.
  9. Click anywhere in the Model Browser to apply these changes.

    os_1392_discret_n2s
    Figure 4. Define the Contact interface

Create Output Requests

In the final step of model preparation, you want to request contact related output, CONTF; which causes Contact Force, Contact Deformation, Contact Status and Contact Traction to be output. Also, CONTPRM,CONTGAP, CONTPRM,CONTGRID and GAPPRM,HMGAPST are used to review the created contact elements.
  1. From the main menu, select Setup > Create > Control Cards.
  2. Select GLOBAL_OUTPUT_REQUEST and CONTF.

    os_1392_global_output_request
    Figure 5. Set up a Global Output Request
  3. In the next panel, select the settings to request contact related output, as shown below.

    os_1392_contf
    Figure 6. Request Contact Related Output
  4. Click return to complete the card definition.
  5. Repeat the steps above to create the CONTGAP and CONTGRID cards, as seen in Figure 7.
    They are available under the CONTPRM control card.
  6. Select UNSUPPORTED_CONTPRMS and enter 2.
  7. Then create the following cards below.
    1. CONTPRM,CONTGAP,YES (outputs the internally created CGAPG for N2S contact)
    2. CONTPRM,CONTGRID,YES (outputs a set containing the grids in S2S contact)
  8. Click return.

    os_1392_contprm
    Figure 7. Define CONTPRM cards CONTGAP and CONTGRID
  9. Click Next to locate the GAPPRM control card and click HMGAPST.
  10. Set the VALUE to YES.
    Outputs the open/closed status of the CGAPG elements.

    os_1392_gapprm_hmgapst
    Figure 8. Define GAPPRM card HMGAPST

Submit the Job

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

    OS_1000_13_17
    Figure 9. Accessing the OptiStruct Panel
  2. Click save as.
  3. In the Save As dialog, specify location to write the OptiStruct model file and enter Contact_N2S for filename.
    For OptiStruct input decks, .fem is the recommended extension.
  4. Click Save.
    The input file field displays the filename and location specified in the Save As dialog.
  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 to launch the OptiStruct job.
If the job is successful, new results files should be in the directory where the Contact_N2S.fem was written. The Contact_N2S.out file is a good place to look for error messages that could help debug the input deck if any errors are present.

Submit a Job for S2S

  1. In the Model Browser, select the top_to_bottom card under Group.
  2. Set DISCRET to S2S.
  3. Repeat the steps in Submit the Job, with the new file name Contact_S2S.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. When the message Process completed successfully is received in the command window, click HyperView.
    HyperView is launched and the results are loaded for the S2S run. A message window appears to verify that the model and result files are loading into HyperView.
  2. Click Close to close the message window, if one appears.
  3. Select the page window layout icon pageLayout2Vertical-24 to split the page into two windows.
  4. Load the other model in the new window by clicking fileImportModel-24 and selecting contact_N2S.h3d.
  5. Click the Contour toolbar icon resultsContour-16 in one of the two windows.
  6. For Result type, select Contact Traction/Normal(s).
  7. Click Apply.

    os_1392_contour_plot
    Figure 10. Contour Plot Panel in HyperView
  8. In the Model Browser, unselect the top part of the structure.
    Only the results on the contact surface are visible.

    os_1392_top_unselect
    Figure 11. Isolate the Bottom Part of the Structure in HyperView
  9. 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.
    A contour plot of normal contact traction shows for both runs. The traction for the S2S run is much more uniform than for N2S by comparing the maximum and minimum values.

    os_1392_apply_style_menu
    Figure 12. Apply the Setup in One Window to the Rest of the Page

    os_1392_contour_s2s_n2s
    Figure 13. Contour of the Normal Contact Traction for S2S on the Left and N2S on the Right

Review the Internally Created CGAPC Elements

After viewing the contact traction in HyperView, check the internally created contact elements for the N2S.
  1. Repeat Steps 1.1 through 1.4.
  2. Select the Contact_N2S.fem file, located in the folder selected in Step 1.4.
  3. Import the internally created CGAPG elements by importing the file contact_N2S.contgap.fem.
  4. Right-click on the component Gaps from CONTACT1 in the Model Browser to review the gap elements.
  5. Select isolate only to visualize the elements better.
  6. Click icon_abc to turn on the element tags.
  7. Click File > Run > Command File to create element sets to identify the open/closed status of the elements at the end of the run.
  8. Select the file contact_N2S.HM.gapstat.tcl.
  9. Run a command file in HyperMesh to create sets containing open and closed gaps.
  10. To see which gaps are closed or open at the end of the simulation, review the element sets that were created. Review the set OS_gaps_sub_001_closed by selecting it in the Model Browser and clicking on the field next to Entity IDs in the Entity State Browser.
    This shows that all gaps are closed, as it contains all elements. If there were some open gaps, another set OS_gaps_sub_001_open would have been created, as well.

    os_1392_review_closed_gaps
    Figure 14. Review the Closed Gaps at the End of the Analysis

Review the Grids

The contact for S2S contact is different from N2S in the sense that no CGAPG elements are created internally. This means the process in Step 8 cannot be applied to S2S contacts. However, you can review the main and secondary grids that are being used in the S2S contact, to ensure that the contact has been established in the correct manner.
  1. Repeat Steps 1.1 through 1.4.
  2. Select the Contact_S2S.fem file, located in the folder selected in Step 1.4.
  3. Import the grid set that show the grids where S2S contact has been established by importing the file contact_S2S.contgrid.fem.
  4. Right-click on the component bottom in the Model Browser and select isolate only to review the grids.
  5. Select Tools > Set Browser.
    The Set Browser opens.
  6. In the Set Browser, right-click on the set ^SecondGrids_Contact_#1 and select Show.
    Contact has been established on the entire surface as expected.

    os_1392_review_slave_nodes
    Figure 15. Review the Secondary Nodes of the S2S Contact
  7. Repeat the steps in Review the Internally Created CGAPC Elements for the component top and the set ^MainGrids_Contact_#1.

Review the Contact Status

The contact status for both N2S and S2S can also be reviewed in HyperView, if the model contained the contact result output request CONTF. To view this, repeat the steps in Compare the Contact Traction while choosing Contact Status/Normal(s) as the contour plot.

os_1392_contour_plot_hv
Figure 16. Review the Contact Status in HyperView as a Contour Plot