Specifying surface property assignments for general contact

Attributes for a general contact interaction, such as surface properties, are specified independently of the contact domain in the Attribute Assignments portion of the interaction editor. For a brief overview of general contact, see Understanding interactions. For a more detailed discussion, see Surface Properties for General Contact in Abaqus/Standard, and Assigning Surface Properties for General Contact in Abaqus/Explicit.

You can specify the following surface properties in a general contact interaction:

  • Surface thickness assignments. Assign nondefault surface thicknesses to shell or membrane surfaces.

  • Shell/Membrane offset assignments. Assign the surface offset to define the distance (as a fraction of the surface thickness) from the midsurface to the reference surface.

  • Surface smoothing assignments. Assign nondefault contact smoothing to model surfaces. Contact smoothing improves the contact stress and pressure accuracy for curved surfaces (see Smoothing Contact Surfaces in Abaqus/Standard).

  • Feature edge criteria assignments. Control the feature edges to be included in the general contact domain. Feature edges of a model include shell perimeter edges and geometric feature edges. Modeling of edge-to-edge contact is not allowed for Abaqus/Standard analyses.

  • Crush Trigger assignments. Control the crushing behaviors relating to CZone methodology in the general contact domain. CZone is an Abaqus/Explicit capability that integrates material, element, and contact modeling aspects to simulate crushing of laminated composites due to contact with other bodies (see CZone Analysis). Modeling of crush trigger contact is not allowed for Abaqus/Standard analyses.

  • Surface friction assignments. Establish friction coefficients as mathematical combinations of coefficients specified as surface properties. Modeling of friction contact is not allowed for Abaqus/Standard analyses.

  • Surface beam smoothing assignments. Assign nondefault beam smoothing to model surfaces.

  • Surface vertex criteria assignments. Control the vertex-to-surface contact formulation in the general contact domain. Vertex criteria of a model specify the vertex nodes that should be considered by the vertex-to-surface formulation (see Vertex Nodes).

This task shows you how to:

See Also
Interaction editors
Defining general contact
In Other Guides
Surface Properties for General Contact in Abaqus/Standard
Assigning Surface Properties for General Contact in Abaqus/Explicit

Specify surface thickness assignments

  1. Display the general contact interaction editor using one of the following methods:

    • To create a new general contact interaction, follow the instructions in Defining general contact.

    • To edit an existing general contact interaction, select Interaction Edit interaction name from the main menu.

  2. Click the Surface Properties tab in the Attribute Assignments portion of the interaction editor.

    The surface thickness can be modified only for surfaces defined on shells and membranes.

  3. Click next to Surface thickness assignments.

    The Edit Surface Thickness Assignments dialog box appears. By default, when you select a surface from the list or the table, Abaqus/CAE highlights the surface in the viewport; however, highlighting does not apply for (Global), and materials. You can toggle off Highlight selected regions at the bottom of the dialog box to turn off selection highlighting.

  4. Select one or more surfaces and materials from the list of existing surfaces and materials in the column on the left. Select (Global) to assign the shell/membrane thickness to the entire contact domain.

    Tip: You can click to define a new surface and add it to the list. See Creating surfaces, for instructions on defining surfaces.
    Tip: You can click to define a new material and add it to the list. See Creating or editing a material, for instructions on defining materials.

  5. Click the arrows in the middle of the dialog box to transfer your selections to the list of shell/membrane thickness assignments.

    The table on the right side of the dialog box is updated to reflect your selections.

  6. Specify the thickness for each surface and material in the middle column of the Surface Thickness Assignments table.

    • Enter the word ORIGINAL to set the shell/membrane thickness equal to the original shell or membrane thickness (the default);
    • enter the word THINNING to set the shell/membrane thickness equal to the current shell or membrane thickness (this option is available only in Abaqus/Explicit); or
    • specify a value for the shell/membrane thickness.

  7. Optionally, specify a scale factor for any of the shell/membrane thickness assignments in the last column of the Surface Thickness Assignments table.
  8. Repeat the above steps as needed to complete the shell/membrane thickness assignments. If you want to delete thickness assignments, select the rows and click .

    Note:

    The order of assignments might be relevant; when shell/membrane thickness assignments overlap, the last assignment takes precedence.

  9. Click OK to save your selections and to close the Edit Surface Thickness Assignments dialog box.

    The interaction editor reappears with updated information on the number of shell/membrane thickness assignments.

  10. Click OK to create the interaction and to close the editor.

Specify shell/membrane offset assignments

  1. Display the general contact interaction editor using one of the following methods:

    • To create a new general contact interaction, follow the instructions in Defining general contact.

    • To edit an existing general contact interaction, select Interaction Edit interaction name from the main menu.

  2. Click the Surface Properties tab in the Attribute Assignments portion of the interaction editor.

    The surface offset can be modified only for surfaces defined on shells and membranes.

  3. Click next to Shell/Membrane offset assignments.

    The Edit Shell/Membrane Offset Assignments dialog box appears. By default, when you select a surface from the list or the table, Abaqus/CAE highlights the surface in the viewport; however, highlighting does not apply for (Global), and materials. You can toggle off Highlight selected regions at the bottom of the dialog box to turn off selection highlighting.

  4. Select one or more surfaces and materials from the list of existing surfaces and materials in the column on the left. Select (Global) to assign the shell/membrane offset to the entire contact domain.

    Tip: You can click to define a new surface and add it to the list. See Creating surfaces, for instructions on defining surfaces.
    Tip: You can click to define a new material and add it to the list. See Creating or editing a material, for instructions on defining materials.

  5. Click the arrows in the middle of the dialog box to transfer your selections to the list of shell/membrane offset assignments.

    The table on the right side of the dialog box is updated to reflect your selections.

  6. Specify the offset fraction for each surface and material in the second column of the Shell/Membrane Offset Assignments table. The offset fraction defines the distance (as a fraction of the thickness) from the midsurface to the reference surface.

    • Enter the word ORIGINAL to set the shell/membrane offset equal to the original shell or membrane offset (the default).

    • Enter SPOS to specify the top surface of the shell/membrane as the reference surface.

    • Enter SNEG to specify the bottom surface of the shell/membrane as the reference surface.

    • Specify a value between −0.5 (indicates the bottom surface of the shell/membrane) and 0.5 (indicates the top surface of the shell/membrane) for the offset fraction.

  7. Repeat the above steps as needed to complete the shell/membrane offset assignments. If you want to delete offset assignments, select the rows and click .

    Note:

    The order of assignments might be relevant; when shell/membrane offset assignments overlap, the last assignment takes precedence.

  8. Click OK to save your selections and to close the Edit Shell/Membrane Offset Assignments dialog box.

    The interaction editor reappears with updated information on the number of shell/membrane offset assignments.

  9. Click OK to create the interaction and to close the editor.

Specify surface smoothing assignments

  1. Display the general contact interaction editor using one of the following methods:

    • To create a new general contact interaction, follow the instructions in Defining general contact.

    • To edit an existing general contact interaction, select Interaction Edit interaction name from the main menu.

    In an Abaqus/Standard general contact interaction, surface smoothing assignments can be specified only in the initial step. In an Abaqus/Explicit general contact interaction, surface smoothing assignments can be specified or modified in any analysis step.

  2. Click the Surface Properties tab in the Attribute Assignments portion of the interaction editor.
  3. Click next to Surface smoothing assignments.

    The Edit Surface Smoothing Assignments dialog box appears. By default, when you select a surface from the list or the table, Abaqus/CAE highlights the surface in the viewport and displays the detected axis or center of curvature that will be used in the smoothing calculation. You can toggle off Highlight selected regions at the bottom of the dialog box to turn off selection highlighting.

  4. Toggle Automatically assign smoothing for geometric faces to determine whether Abaqus/CAE applies surface smoothing automatically to all appropriate surfaces in the general contact domain. This option is on by default for Abaqus/Standard general contact interactions and off by default for Abaqus/Explicit general contact interactions.
  5. Select one or more surfaces from the list of existing surfaces in the column on the left.

    Tip: You can click to define a new surface and add it to the list. See Creating surfaces, for instructions on defining surfaces.

  6. Click the arrows in the middle of the dialog box to transfer your selections to the list of surface smoothing assignments.

    The table on the right side of the dialog box is updated to reflect your selections.

  7. Specify the smoothing to apply to each surface in the second column of the Surface Smoothing Assignments table. The smoothing specified for these surfaces overrides the default global smoothing if it is applied.

    • Select REVOLUTION to apply circumferential smoothing to a curved surface that is symmetric about an axis of revolution (or a two-dimensional arc that is symmetric about a central point).

    • Select SPHERICAL to apply spherical smoothing to a curved surface that is symmetric about a central point.

    • Select TOROIDAL to apply toroidal smoothing to a curved surface that is a circular arc symmetric about an axis of revolution.

    • Select NONE to prevent smoothing from being applied to the specified surface.

  8. Repeat the above steps as needed to complete the surface smoothing assignments. If you want to delete smoothing assignments, select the rows and click .

    Note:

    The order of assignments might be relevant; when smoothing assignments overlap, the last assignment takes precedence.

  9. Click OK to save your selections and to close the Edit Surface Smoothing Assignments dialog box.

    The interaction editor reappears with updated information on the number of surface smoothing assignments.

  10. Click OK to create the interaction and to close the editor.

Specify feature edge criteria assignments

  1. Display the general contact interaction editor using one of the following methods:

    • To create a new general contact interaction, follow the instructions in Defining general contact.

    • To edit an existing general contact interaction, select Interaction Edit interaction name from the main menu.

  2. Click the Surface Properties tab in the Attribute Assignments portion of the interaction editor.
  3. Click next to Feature edge criteria assignments.

    The Edit Feature Edge Criteria Assignments dialog box appears. By default, when you select a surface from the list or the table, Abaqus/CAE highlights the surface in the viewport; however, highlighting does not apply for (Global), and materials. You can toggle off Highlight selected regions at the bottom of the dialog box to turn off selection highlighting.

  4. Select one or more surfaces and materials from the list of existing surfaces in the first column on the left side of the dialog box. Select (Global) to assign the surface feature to the entire contact domain.

    Tip: You can click to define a new surface and add it to the list. See Creating surfaces, for instructions on defining surfaces.
    Tip: You can click to define a new material and add it to the list. See Creating or editing a material, for instructions on defining materials.

  5. Select the configuration from the second column on the left (this option is available only for Abaqus/Explicit).
  6. Click the arrows in the middle of the dialog box to transfer your selections to the list of surface feature assignments.

    The table on the right side of the dialog box is updated to reflect your selections.

  7. Specify the feature edge criteria for each surface and material in the second and third column of the Surface Feature Assignments table by doing one of the following:

    • Enter the word PERIMETER to include only perimeter edges in the general contact domain.

    • Enter the word ALL to include all edges in the general contact domain (this option is available only for Abaqus/Explicit).

    • Enter the word PICKED to include in the general contact domain only edges that were explicitly selected as part of the surface definition (this option is available only for shell geometries and elements in Abaqus/Explicit).

    • Enter the word NONE to include no feature edges in the general contact domain.

    • Specify an angle in degrees to include perimeter edges and geometric edges with feature angles greater than or equal to the specified angle in the general contact domain. The specified value must be between 0° and 180°. For examples of how the feature angle is calculated for different edges, see Feature Edges.

  8. Repeat the above steps as needed to complete the surface feature assignments. If you want to delete surface feature assignments, select the rows and click .

    Note:

    The order of assignments might be relevant; when surface feature assignments overlap, the last assignment takes precedence.

  9. For an Abaqus/Explicit general contact interaction, toggle Use dynamic feature edges to activate or deactivate the dynamic feature edge criterion for the contact surface.
  10. Click OK to save your selections and to close the Edit Feature Edge Criteria Assignments dialog box.

    The interaction editor reappears with updated information on the number of feature edge criteria assignments.

  11. Click OK to create the interaction and to close the editor.

Specify crush trigger assignments

  1. Display the general contact interaction editor using one of the following methods:

    • To create a new general contact interaction, follow the instructions in Defining general contact.

    • To edit an existing general contact interaction, select Interaction Edit interaction name from the main menu.

  2. Click the Surface Properties tab in the Attribute Assignments portion of the interaction editor.
  3. Click next to Crush trigger assignments.

    The Edit Crush Trigger Assignments dialog box appears. By default, when you select a surface from the list or the table, Abaqus/CAE highlights the surface in the viewport; however, highlighting does not apply for (Global) and materials. You can toggle off Highlight selected regions at the bottom of the dialog box to turn off selection highlighting.

  4. Select one or more surfaces and materials from the list of existing surfaces in the first column on the left side of the dialog box. Select (Global) to assign the surface feature to the entire contact domain.

    Tip: You can click to define a new surface and add it to the list. See Creating surfaces, for instructions on defining surfaces.
    Tip: You can click to define a new material and add it to the list. See Creating or editing a material, for instructions on defining materials.

  5. Click the arrows in the middle of the dialog box to transfer your selections to the list of crush trigger assignments.

    The table on the right side of the dialog box is updated to reflect your selections.

  6. Specify the trigger option for each surface and material in the second column of the Crush Trigger Assignments table by doing one of the following:

    • Enter the word TRIGGER to specify that node develops contact pressures consistent with the assigned contact pressure-overclosure relationship.

    • Enter the word NO_TRIGGER to specify that nodes will be reassigned trigger status during the simulation if adjacent nodes begin crushing or adjacent elements experience material failure.

    • Enter the word NO_CRUSH to specify that the nodes have no crush associated with adjacent elements and will never crush.

  7. Specify the crush stress, crush initiation angle, and crush continuation angle for each surface and material in the third, fourth, and fifth columns of the Crush Trigger Assignments table by doing the following:

    • Specify a scalar value representing the stress required to initiate crushable behavior as a factor of the crush stress in column Crush Stress.

    • Specify an angle in degrees representing crush initiation angle.

    • Specify an angle in degrees representing crush continuation angle.

  8. Repeat the above steps as needed to complete the crush trigger assignments. If you want to delete crush trigger assignments, select the rows and click .

    Note:

    The order of assignments might be relevant; when crush trigger assignments overlap, the last assignment takes precedence.

  9. Click OK to save your selections and to close the Edit Crush Trigger Assignments dialog box.

    The interaction editor reappears with updated information on the number of crush trigger assignments.

  10. Click OK to create the interaction and to close the editor.

Specify surface friction assignments

  1. Display the general contact interaction editor using one of the following methods:

    • To create a new general contact interaction, follow the instructions in Defining general contact.

    • To edit an existing general contact interaction, select Interaction Edit interaction name from the main menu.

  2. Click the Surface Properties tab in the Attribute Assignments portion of the interaction editor.
  3. Click next to Surface friction assignments.

    The Edit Surface Friction Assignments dialog box appears. By default, when you select a surface from the list or the table, Abaqus/CAE highlights the surface in the viewport; however, highlighting does not apply for (Global) and materials. You can toggle off Highlight selected regions at the bottom of the dialog box to turn off selection highlighting.

  4. Select one or more surfaces and materials from the list of existing surfaces and materials in the column on the left. Select (Global) to assign the surface-based friction coefficient to the entire contact domain.

    Tip: You can click to define a new surface and add it to the list. See Creating surfaces, for instructions on defining surfaces.
    Tip: You can click to define a new material and add it to the list. See Creating or editing a material, for instructions on defining materials.

  5. Click the arrows in the middle of the dialog box to transfer your selections to the list of surface friction assignments.

    The table on the right side of the dialog box is updated to reflect your selections.

  6. Specify the surface-based friction coefficients for each surface and material in the second column of the Surface Friction Assignments table.
  7. Repeat the above steps as needed to complete the surface friction assignments. If you want to delete surface friction assignments, select the rows and click .

    Note:

    The order of assignments might be relevant; when surface friction assignments overlap, the last assignment takes precedence.

  8. Click OK to save your selections and to close the Edit Surface Friction Assignments dialog box.

    The interaction editor reappears with updated information on the number of surface friction assignments.

  9. Click OK to create the interaction and to close the editor.

Specify surface beam smoothing assignments

  1. Display the general contact interaction editor using one of the following methods:

    • To create a new general contact interaction, follow the instructions in Defining general contact.

    • To edit an existing general contact interaction, select Interaction Edit interaction name from the main menu.

  2. Click the Surface Properties tab in the Attribute Assignments portion of the interaction editor.
  3. Click next to Surface beam smoothing assignments.

    The Edit Beam Smoothing Assignments dialog box appears. By default, when you select a surface from the list or the table, Abaqus/CAE highlights the surface in the viewport and displays the detected axis or center of curvature that is used in the smoothing calculation. You can toggle off Highlight selected regions at the bottom of the dialog box to turn off selection highlighting.

  4. Select one or more surfaces from the list of existing surfaces in the column on the left.

    Tip: You can click to define a new surface and add it to the list. See Creating surfaces, for instructions on defining surfaces.

  5. Click the arrows in the middle of the dialog box to transfer your selections to the list of beam smoothing assignments.

    The table on the right side of the dialog box is updated to reflect your selections.

  6. Specify the smoothing to apply to each surface in the second column of the Beam Smoothing Assignments table. The smoothing specified for these surfaces overrides the default global smoothing if it is applied.

    Specify a value between 0.0 and 0.5 for the beam smoothing.

  7. Repeat the above steps as needed to complete the beam smoothing assignments. If you want to delete beam smoothing assignments, select the rows and click .

    Note:

    The order of assignments might be relevant; when beam smoothing assignments overlap, the last assignment takes precedence.

  8. Click OK to save your selections and to close the Edit Beam Smoothing Assignments dialog box.

    The interaction editor reappears with updated information on the number of beam smoothing assignments.

  9. Click OK to create the interaction and to close the editor.

Specify surface vertex criteria assignments

  1. Display the general contact interaction editor using one of the following methods:

    • To create a new general contact interaction, follow the instructions in Defining general contact.

    • To edit an existing general contact interaction, select Interaction Edit interaction name from the main menu.

  2. Click the Surface Properties tab in the Attribute Assignments portion of the interaction editor.
  3. Click next to Surface vertex criteria assignments.

    The Edit Vertex Criteria Assignments dialog box appears. By default, when you select a surface from the list or the table, Abaqus/CAE highlights the surface in the viewport; however, highlighting does not apply for (Global) and materials. You can toggle off Highlight selected regions at the bottom of the dialog box to turn off selection highlighting.

  4. Select one or more surfaces and materials from the list of existing surfaces in the first column on the left side of the dialog box. Select (Global) to assign the surface feature to the entire contact domain.

    Tip: You can click to define a new surface and add it to the list. See Creating surfaces, for instructions on defining surfaces.
    Tip: You can click to define a new material and add it to the list. See Creating or editing a material, for instructions on defining materials.

  5. Click the arrows in the middle of the dialog box to transfer your selections to the list of vertex criteria assignments.

    The table on the right side of the dialog box is updated to reflect your selections.

  6. Specify the vertex criteria for each surface and material in the second column of the Vertex Criteria Assignments table by doing one of the following:

    • Enter the word ALL_VERTICES to specify that all vertex nodes should be considered by the vertex-to-surface formulation.

    • Enter the word NO_VERTICES to specify that no vertex nodes should be considered by the vertex-to-surface formulation.

    • Specify an angle in degrees representing the vertex angle threshold. The specified value must be between 10° and 90°.

  7. Repeat the above steps as needed to complete the vertex criteria assignments. If you want to delete vertex criteria assignments, select the rows and click .

    Note:

    The order of assignments might be relevant; when vertex criteria assignments overlap, the last assignment takes precedence.

  8. Click OK to save your selections and to close the Edit Vertex Criteria Assignments dialog box.

    The interaction editor reappears with updated information on the number of vertex criteria assignments.

  9. Click OK to create the interaction and to close the editor.