Defining surface-to-surface contact in an Abaqus/Standard analysis

Certain interaction behaviors can be defined in Abaqus/Standard only by using surface-to-surface contact; see Contact simulation capabilities in Abaqus/Standard for more information.

Related Topics
Interaction editors
Customizing contact controls
In Other Guides
About contact pairs in Abaqus/Standard

  1. From the main menu bar, select InteractionCreate.

    Tip: You can also create a surface-to-surface contact interaction using the tool in the Interaction module toolbox.

  2. In the Create Interaction dialog box that appears, do the following:

    • Name the interaction. For more information about naming objects, see Using basic dialog box components.

    • Select the step in which the interaction will be created.

    • Select the Surface-to-surface contact (Standard) type of interaction.

  3. Click Continue to close the Create Interaction dialog box.

  4. Use one of the following methods to select the master surface:

    • Use an existing surface to define the region. On the right side of the prompt area, click Surfaces. Select an existing surface from the Region Selection dialog box that appears, and click Continue.

      Note:

      The default selection method is based on the selection method you most recently employed. To revert to the other method, click Select in Viewport or Surfaces on the right side of the prompt area.

    • Use the mouse to select a region in the viewport. (For more information, see Selecting objects within the current viewport.) Click mouse button 2 to indicate you have finished selecting. Certain connectivity restrictions apply to contact surfaces depending on the type of contact formulation. For detailed information, see About contact pairs in Abaqus/Standard.

      If the model contains a combination of mesh and geometry, click one of the following from the prompt area:

      • Click Geometry if you want to select the surface from a geometry region.

      • Click Mesh if you want to select the surface from a native or orphan mesh selection.

      You can use the angle method to select a group of faces or edges from geometry or a group of element faces from a mesh. For more information, see Using the angle and feature edge method to select multiple objects.

    The master surface that you select becomes highlighted in red in the viewport.

  5. Select the slave surface.

    1. In the prompt area, select one of the following:

      • Select Surface if you want to select a surface.

      • Select Node Region if you want to select a region from which to create a contact node set.

    2. Use one of the same methods described earlier to select the slave surface or region.

      The slave surface or region that you select becomes highlighted in magenta in the viewport.

      The Edit Interaction dialog box appears.

  6. The Switch Surfaces option allows you to interchange your master and slave surface selections without having to start over. The Switch Surfaces icon is available only if you selected Surface in the previous step.

  7. Choose the sliding formulation.

    • Choose Finite sliding to use the finite-sliding formulation, which is the most general and allows any arbitrary motion of the surfaces.

    • Choose Small sliding to use the small-sliding formulation, which assumes that although two bodies may undergo large motions, there will be relatively little sliding of one surface along the other.

    For more information, see Contact formulations in Abaqus/Standard.

  8. Select the discretization method.

    • Select Node to surface to use the node-to-surface discretization method.

    • Select Surface to surface to use the surface-to-surface discretization method.

    For more information, see Discretization of contact pair surfaces.

  9. Different fields become available depending upon the combination of your sliding formulation and discretization method selections.

    • By default, shell and membrane thicknesses are included in contact calculations for the following combinations: Small sliding and Node to surface, Small sliding and Surface to surface, and Finite sliding and Surface to surface. You can toggle on Exclude shell/membrane element thickness to ignore shell and membrane thickness for any of these combinations.

      Contact interactions using Finite sliding and Node to surface do not account for surface thickness. For more information, see Accounting for shell and membrane thickness.

    • For contact interactions using the Node to surface discretization method, you can specify a smoothing factor in the Degree of smoothing for master surface field. For more information, see Smoothing master surfaces for the finite-sliding, node-to-surface formulation.

    • By default, a selective scheme of supplementary contact constraints is used for the following combinations: Finite sliding and Node to surface, Small sliding and Node to surface, and Small sliding and Surface to surface. For these combinations, you can specify when to Use supplementary contact points as follows:

      • Choose Selectively to use a selective scheme of supplementary contact constraints.

      • Choose Never to forgo the use of supplementary contact constraints.

      • Choose Always to add supplementary contact constraints when applicable.

      For more information, see Supplementary contact constraints.

    • For contact interactions using Finite sliding and Surface to surface, you can choose the Contact tracking method.

      • Choose Single configuration (state) to use the state-based tracking algorithm.

      • Choose Two configurations (path) to use the path-based tracking algorithm.

      For more information, see Path-based versus state-based tracking algorithms.

      Note:

      If your contact interaction uses the surface-to-surface discretization method and one or more of the surfaces in the contact interaction is an analytical rigid surface, you should choose the state-based tracking algorithm.

  10. Specify the slave node adjustment option. For more information, see Adjusting initial surface positions and specifying initial clearances in Abaqus/Standard contact pairs and Defining tied contact in Abaqus/Standard.

  11. For contact interactions using the Surface to surface discretization method, you can apply a smoothing to contacting surfaces that reduces inaccuracies in contact pressures caused by mesh discretization on curved geometries. Click the Surface Smoothing tab, and select one of the following options:

    • Choose Do not smooth to prevent smoothing from being applied.

    • Choose Automatically smooth 3D geometry surfaces when applicable to apply smoothing to axisymmetric or spherical surfaces (or portions of surfaces) that are identified automatically by Abaqus/CAE. Automatic smoothing has no effect on mesh parts or two-dimensional models.

    For more information about contact smoothing techniques, see Smoothing contact surfaces in Abaqus/Standard.

  12. For contact interactions using the Small sliding formulation, you can specify an initial clearance between the nodes on the slave surface and the master surface. Click the Clearance tab, select a clearance type from the Initial clearance field, and enter all of the data necessary to define the clearance and contact direction. For more information, see Defining a precise initial clearance or overclosure for small-sliding contact.

  13. If you specify node-to-surface discretization for your contact interaction, you can also limit bonding to slave nodes in a particular subset. Click the Bonding tab, toggle on Limit bonding to slave nodes in subset, and select a node set from the list.

    You can limit bonding for either of the following:

    • When you want to specify a subset of initially slave nodes that should experience cohesive forces. Strain-free adjustments will be made for those nodes initially not in contact but specified in the node set. All slave nodes outside of this set (including those that are initially contacting the master surface) will experience only compressive contact forces over the course of the analysis. For more information, see Specifying cohesive behavior properties for mechanical contact property options.

    • When you want to identify the initially bonded region of the slave surface in a VCCT crack. The unbonded portion of the slave surface behaves as a regular contact surface. The predetermined crack surfaces are assumed to be initially partially bonded so that the crack tips can be identified explicitly during the analysis. For more information, see Defining initially bonded crack surfaces in Abaqus/Standard.

  14. Select a contact interaction property. If desired, click to create the interaction property.

    For more information, see Defining a contact interaction property and Contact constraint enforcement methods in Abaqus/Standard.

  15. To specify interference fit options, click Interference Fit. Interference fit options cannot be specified in the initial step. See Specifying interference fit options below for more detailed instructions on entering interference fit options.

  16. If desired, click the arrow next to the Contact controls field and select the customized contact controls to use for this interaction. Only previously created Abaqus/Standard contact controls appear in the list. For more information, see Specifying contact controls in an Abaqus/Standard analysis.

  17. To deactivate and reactivate a contact interaction in a step, toggle Active in this step. The contact interaction is active in the step in which it was created. For more information, see Removing and reactivating contact pairs.

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