Products: Abaqus/Standard Abaqus/CAE
“Defining surface-to-surface contact,” Section 15.13.6 of the Abaqus/CAE User's Manual
“Defining self-contact,” Section 15.13.7 of the Abaqus/CAE User's Manual
This section describes how to modify the properties associated with surfaces in a contact pair definition.
All of the contact formulations except the finite-sliding, node-to-surface formulation account for initial shell and membrane thicknesses for element-based surfaces by default. The finite-sliding, node-to-surface formulation will not account for surface thickness. Node-based surfaces have no thickness, regardless of which element types are connected to the surface nodes. Accounting for element thicknesses in contact calculations is generally desirable, but you can avoid having thickness considered if it is not desired.
| Input File Usage: | *CONTACT PAIR, NO THICKNESS |
| Abaqus/CAE Usage: | Interaction module: interaction editor: Sliding formulation: Small sliding or Finite sliding, Discretization method: Surface to surface or Node to surface, toggle on Exclude shell/membrane element thickness |
Consider the case of a shell pinched between two rigid surfaces, as shown in Figure 34.3.2–1.
In this example contact pairs using the small-sliding, node-to-surface formulation are defined between the top surface of the shell and the top rigid surface and between the bottom surface of the shell and the bottom rigid surface. Although the shell surfaces are defined at the shell reference location, the contact interactions account for the thickness of the shell and are offset from the reference surface. The penalty constraint enforcement method (see “Contact pressure-overclosure relationships,” Section 35.1.2) is used to avoid overconstraining slave nodes. The following input is used:
*SURFACE, NAME=TOP_RIG_SURF TOP_RIG_ELS, *SURFACE, NAME=SHELL_TOP_SURF SHELL_ELS,SPOS *SURFACE, NAME=SHELL_BOT_SURF SHELL_ELS,SNEG *SURFACE, NAME=BOT_RIG_SURF BOT_RIG_ELS, *CONTACT PAIR, INTERACTION=INTER_AL, SMALL SLIDING SHELL_TOP_SURF, TOP_RIG_SURF SHELL_BOT_SURF, BOT_RIG_SURF *SURFACE INTERACTION, NAME=INTER_AL *SURFACE BEHAVIOR, PENALTY
With the finite element method, curved geometric surfaces are naturally approximated as a faceted group of connected element faces. The use of a faceted surface geometry rather than the true surface geometry can significantly contribute to contact stress inaccuracy in contact pairs, especially when the magnitude of the differences between the faceted and true surface is not small with respect to the deformation of the components in contact. Methods for overcoming convergence and accuracy difficulties associated with faceted surfaces in contact interactions are discussed in “Contact formulations in Abaqus/Standard,” Section 36.1.1, and “Smoothing contact surfaces in Abaqus/Standard,” Section 36.1.3.
