Contacts

Contacts indicate whether neighboring surfaces should be bonded, contacting, or have no contact.

This tool detects possible contacts in your model. If contacts aren't found, you can manually create contacts between parts.



Click the satellite icon that appears when you hover over the Contacts tool to view a list of all contacts in your model.


Figure 1. Model with Contacts Defined

Defining Surface Contacts

Find neighboring surfaces and designate whether they should be bonded, contacting, or have no contact.

  1. On the Structures ribbon, select the Contacts tool.
  2. Select Surfaces on the guide bar.

  3. Click the Find button.
    Bonded contacts are shown in blue; contacting in green.
  4. Select a contact to redefine, and change its type in the microdialog.

  5. To redefine all contacts of the same type:
    1. Click the Auto button on the guide bar and select Bonded, Contacting, or No Contact from the list.
    2. Click Redefine All to apply changes to the entire group.

  6. Right-click and mouse through the check mark to exit, or double-right-click.
Tip:
  • To automatically detect relevant features when the tool is opened, go to the Preferences under Inspire > Geometry and turn on Autofind.
  • If a contact is not detected, try changing the Auto Search Distance under the Find Options on the guide bar.
  • Inspire detects contact between surfaces and solids, but not all cases are considered valid. (View examples of valid and invalid contacts later in this topic).
  • If Auto is selected on the guide bar, Inspire automatically determines whether contacts should be bonded or contacting based on the presence of other connections between parts. If there are no fasteners or joints connecting two parts together, they are assumed to be bonded. If fasteners or joints are present, parts are assumed to be contacting.
  • Two parts which are in contact in multiple locations must have the same type of contact at each location.
  • OptiStruct analysis supports both surface-to-surface and node-to-surface type contacts.

Defining Part-to-Part Contacts

Create contacts between parts manually.

  1. On the Structures ribbon, select the Contacts tool.
  2. Select Parts on the guide bar.

  3. Click the Find button.
    Bonded contacts are shown in blue; contacting in green.
  4. Select two parts.
  5. Click Define on the guide bar, or click on the selected red parts to define the contact. Part-to-part contacts are automatically defined as bonded.
  6. Select Bonded, Contacting, or No Contact in the microdialog.

  7. Right-click and mouse through the check mark to exit, or double-right-click.
Note:
  • If a contact is not detected, try changing the Auto Search Distance under the Find Options on the guide bar.
  • Inspire detects contact between surfaces and solids, but not all cases are considered valid. (View examples of valid and invalid contacts later in this topic)

Microdialog Options

Click a selected contact to open a microdialog and change the type. The options are Bonded, Contacting, or No Contact.



  • Select Bonded if parts are bonded or glued together.
  • Select Contacting if there is relative sliding between the parts.
  • Select No Contact if parts are close but you don't want them to have contact.

Auto Search Distance

The auto search distance is a global search threshold that uses default tolerances to find locations where joints can be created.

Click the Find Options menu on the guide bar to change the Auto search distance. When the checkbox is enabled, it is calculated automatically.



To change the search distance, deselect the checkbox and enter a value in the text box. Any contacts with a minimum gap less than the entered search distance will be found. (The minimum gap is the exact minimum distance between the two parts.)



Figure 2. Auto Search Distance

The minimum separation between the beam and the blocks in this model ranges from 0.0 to 0.06 mm. When the search distance is manually set to 0.03 mm, the first four contacts with a minimum separation of 0.03 mm or less are detected.

Fixing Disconnected Groups

Find and review any disconnected groups of parts using the Disconnected Groups tool on the Contacts icon.

Contacts are defined differently depending on which solver you use. With the OptiStruct solver, contacts are defined between parts; with SimSolid they are defined between faces, which may result in a greater number of contacts. If you switch between solvers, you will need to open the Contacts tool, click Find, and then redefine contacts using the appropriate method.



You can find and review any disconnected groups of parts using the Disconnected Groups tool on the Contacts icon.



Note: This tool only appears when the SimSolid solver has been enabled in the Preferences.

Defining Contacts for Optimization

When running an optimization, you must designate whether contacts should slide, or slide and separate.

The type of contacts you create will have an impact on analysis and optimization calculations, as bonded and contacting parts create different load paths. Also note that parts which are contacting may either slide, or slide and separate. Allowing separation can have a significant impact on optimization run times, so you may designate Sliding only or Sliding with separation under Contacts on the Run Optimization window. If there are no contacting parts in your model, this option will be grayed out.


Contacts Table

The Contacts table lists all of the contacts in your model including the type of connection and the parts it connects.

Click the satellite icon on the Contacts tool to display the table.



The Search Distance listed in the Contacts table shows the minimum gap (the exact minimum distance between the two parts). The search distance for an individual contact defined in this table will override the global Auto search distance defined in the Find Options on the guide bar.

The table data can be edited with the following actions:

To Do this
Rename a contact Select the cell in the table and then click again to make the field editable.
Change the connection type Select the cell in the table and then select a different option from the list.
Sort a column Click the column header. Click repeatedly to toggle between ascending and descending order.
Add or remove columns Right-click on a column header.

Contact Clearance

Contact clearance is an advanced feature used to either force or prevent contact in cases where there is a slight separation between contacting parts. It is only considered when running an analysis or optimization with the Sliding with Separation option selected.

By default, the contact clearance is set to 0.0, meaning that the parts are always in contact regardless of the minimum separation. You can change the default value by clicking the icon on the Contacts guide bar.

To edit the contact clearance for an indivudal contact:

  1. Click the List Contacts satellite icon on the Contacts tool.
  2. Right-click a column header on the Contacts Table and select Clearance to add it to the table.


  3. Enter a Clearance for the desired contact in the table. To enforce a contact from the beginning of the solution, set the contact clearance to 0.0. If you want the parts to operate independently and only contact if they physically touch during the load case, remove 0.0 and set the value to (none). To enforce an interference fit, enter a positive clearance. To add clearance between touching parts, enter a negative value into the contact clearance field.


Figure 3. Original Model. There is a 0.5 mm gap between the button and the corresponding contacting part.


Figure 4. No Contact. Deflection is < 0.5 mm, so no contact occurs.


Figure 5. Contact. Deflection is > 0.5 mm, so contact occurs between the parts.


Figure 6. Enforced Contact. Contact is enforced between the parts when clearance is 0.0.

Mouse Controls and Keyboard Shortcuts

To Do this
Select a contact Left-click a contact to select it.
Select multiple contacts Hold down the Ctrl key and left-click, or use box selection.
Deselect contacts Hold down the Ctrl key and left-click a selected contact.
Deselect all contacts Left-click on an empty space in the modeling window.
Delete part contacts Select a manually defined part contact in the Contacts table and click Delete.
Exit the tool Right-click and mouse through the check mark to exit, or double-right-click.

Valid and Invalid Contacts

Inspire detects contact between surfaces and solids, but not all cases are considered valid.

The following are examples of valid contacts:
Geometry Valid Contact Description Type




Exact Surface Edge to Surface Face Surface or Part-to-Part




Surface Intersection Surface or Part-to-Part




Exact Surface Edge to Exact Surface Edge Surface or Part-to-Part




Overlapping Surfaces Surface or Part-to-Part




Surface to Midsurface Surface or Part-to-Part




Overlapping Surface and Solid Surface or Part-to-Part




Solid to Midsurface Surface or Part-to-Part




Exact Surface Edge to Exact Solid Edge Surface or Part-to-Part




Surface to Surface at a Distance Part-to-Part only




Surface to Solid at a Distance Part-to-Part only




Solid to Solid at a Distance Part-to-Part only
The following are examples of invalid contacts:
Geometry Invalid Contact Description




Surface and Solid Intersection




Exact Solid Edge to Exact Solid Edge