Defining General Contact in Explicit Dynamic Steps

You can apply general contact for a fast and efficient method to specify contact behavior between many or all components in a model.

While defining general contact, you might need to specify a surface pair to make assignments. The app provides you with a context toolbar that contains options to help you select your supports. The supports can be either surfaces or beams, but one support cannot contain a mix of both element types.

The app highlights the surfaces that you select. Surfaces that belong to the main support (Surface 1) appear green, while surfaces that you select that belong to the secondary support (Surface 2) appear magenta. You can click the green button to display the parts that are associated with Surface 1 only. Similarly, you can click the magenta button to display the parts that are associated with Surface 2 only.

You can define only one general contact behavior in a simulation scenario.

Before you begin:
See Also
About General Contact
Defining Contact Properties in Structural Steps
Defining Contact Initialization
Defining Surface-Based Contact in Explicit Dynamic Steps
In Other Guides
About Step-dependent Actions
  1. From the Interactions section of the action bar, click General Contact .
  2. Optional: Enter a descriptive Name.
  3. From the Included surface pairs options, select one of the following:
    OptionDescription
    All surfaces Enforces general contact for all surface pairs, unless you define the Specify excluded surfaces and Surface exclusions options.
    Specified surfaces Enforces general contact only for the surface pairs in Surface inclusions.
  4. If you selected Specified surfaces, select the surface pairs for which to assign the general contact definition.
    1. Expand the Surface inclusions section, and click Create inclusion.
    2. Select the supports for Surface 1 and Surface 2.
    3. Click OK.

    You can repeat the above steps to include more surface pairs.

    The dialog box displays a table that shows the included surface pairs. You can select a row in the table to highlight the corresponding surfaces in the model.
  5. Optional: Select Specify excluded surfaces to remove specific surface pairs from the general contact definition.
    1. Expand the Surface exclusions section, and click Create exclusion.
    2. Select the supports for Surface 1 and Surface 2.
    3. Click OK.

    You can repeat the above steps to exclude more surface pairs.

    The dialog box displays a table that shows the excluded surface pairs. You can select a row in the table to highlight the corresponding surfaces in the model.
  6. Select Apply geometry-based corrections to apply CAD-based surface smoothing to the contacting surfaces to improve the accuracy and robustness of the simulation.

    Surface smoothing can reduce stress noise and contact pressure noise in the results, providing a more uniform and accurate solution.

  7. From the Global contact property options, select a contact property to define the general contact behavior for the simulation.

    If you do not choose a specific property, the app applies (Default penalty contact). This contact mode equates to a linear penalty method of surface behavior. For more information, see Contact Constraint Enforcement Methods in Abaqus/Standard.

    Note: (Default penalty contact) is different from the behavior defined by an "empty" contact property (with no options selected).

  8. Optional: Override the global contact property, and assign custom contact properties to specific surface pairs.
    1. Expand the Contact property assignments section, and click Create property assignment.
    2. Select the supports for Surface 1 and Surface 2.

      Supports can be either surfaces or beams, but one support cannot contain a mix of both element types.

    3. From the Contact property options, select a contact property to assign to the surface pair.
    4. Click OK.

    The app ignores any assignments that you make to surface pairs that are not included in the general contact definition.

  9. Optional: Assign contact initialization definitions to correct small gaps or overclosures for specific surface pairs.
    1. Expand the Contact initialization assignments section, and click Create initialization assignment.
    2. Select the surface supports for Surface 1 and Surface 2.
    3. If the supports include shell geometry, verify that you have applied the contact interaction on the correct side of the surface.

      Tip: You can click to change the side.

    4. From the Contact initialization options, select a contact initialization type to associate with the surface pair.
    5. Click OK.

    The app ignores any assignments that you make to surface pairs that are not included in the general contact definition.

  10. Optional: Assign edge criteria definitions to specific surfaces.
    1. Expand the Edge criteria assignments section, and click Create edge criteria assignment.
    2. Select surfaces or beams as the support.
    3. Specify whether the edge criteria is applied Statically or Dynamically.
    4. Select a Primary edge criteria from the list.
    5. If you chose Angle (primary feature cutoff angle) in the previous step, specify a value.
    6. Select a Secondary edge criteria from the list.
    7. If you chose Angle (secondary feature cutoff angle) in the previous step, specify a value.
    8. Click OK.

    The app ignores any assignments that you make to surfaces that are not included in the general contact definition.

  11. Optional: Assign thickness definitions to specific surfaces.
    1. Expand the Thickness assignments section, and click Create thickness assignment.
    2. Select surfaces or beams as the support.
    3. Select an option from the Thickness list.
    4. If you selected Value, specify a thickness value.
    5. Enter a value for the Scale factor, which the app uses to scale the thickness value.
    6. Click OK.

    The app ignores any assignments that you make to surfaces that are not included in the general contact definition.

  12. Optional: Assign controls definitions to specific surface pairs.
    1. Expand the Controls assignments section, and click Create controls assignment.
    2. From the Type options, select one of the following:

      Option Description
      Contact thickness reduction Eliminates thickness reductions in regions of the model that are excluded from self-contact.
      Scale penalty stiffness Assigns penalty stiffness scale factors to different regions.

    3. If you chose Contact thickness reduction, select Include shell perimeters to reduce the thickness at shell perimeters where perimeter offsets are insufficient to avoid the “bull-nose” effect.
    4. If you chose Scale penalty stiffness, select the supports for Surface 1 and Surface 2, and specify the penalty Scale factor.
    5. Click OK.

    The app ignores any assignments that you make to surfaces that are not included in the general contact definition.

  13. Click OK.