Contact Pairs
Selecting Source and Destination
To decide which boundaries to assign as source and destination in a contact pair, consider the following guidelines:
•
If there is a significant difference in the stiffness in the normal direction between the source and destination boundaries, select the stiffer side as source. This is especially important if the difference in stiffness is quite large (for example, more than a factor of ten).
•
When the contacting parts have approximately the same stiffness, consider the geometry of the boundaries instead. Make a concave boundary the source and a convex boundary the destination rather than the opposite.
•
If one of the boundaries belongs to a part that is rigid it should be selected as the source boundary. Rigid boundaries can be created in several ways, for example
-
The underlying domain has a Rigid Domain material model.
-
The boundary or its underlying domain is constrained by, for example, Fixed Constraint or Prescribed Displacement.
-
The source boundary is meshed, but has no physics attached.
-
The source boundary position is controlled by Prescribed Deformation under Moving Mesh.
•
If only one side of the contact pair is within the physics interface to which the Contact node is added, that must be the destination side.
•
If you are modeling contact between a Shell interface and something else, the Shell interface should be on the destination side. Another way to state this is that the Contact node should be added to the Shell interface. The same principle applies to the Layered Shell and Membrane interfaces.
For efficiency, include only those boundaries that can potentially come in contact in the destination selection. All equations are formed on the destination boundary, and includes performing the contact search which can be expensive.
When making the source selection, you can improve efficiency by selecting a region such that every point on the destination ‘sees’ a corresponding source point. The search follows the normal from the destination boundary. The search will be faster if a point on the source is found than if it is not, even if this point will never come into contact.
Strategies for Selecting Contact Pairs
A Contact node can reference any number of contact pairs.
A contact pair is just a definition, and does not have to be referenced by any Contact node.
Neither the source, nor the destination, in a contact pair has to be geometrically contiguous. In practice, this means that you often only need a few contact pairs in a model. The number of pairs actually needed will be determined by how many different settings that are required in the Contact Pair and Contact nodes.
If you have many contact pairs in your model, it is a good idea to manually set the Label of each pair in order to simplify the identification during subsequent selections in the Contact nodes.
Automatic Generation of Contact Pairs
Contact pairs can be automatically generated during the finalization of the geometry sequence. When Action is set to Form an assembly, you can select Create pairs, and use Contact pair as Pair type. Boundaries which are in geometrical contact with each other will then be placed in contact pairs. When you add Contact nodes in the physics interface, you select which of these suggested pairs to actually use for the contact analysis.
The automatic pair generation will not know which side to use as source or destination. Based on the suggestions in Selecting Source and Destination above, you may need to switch selections using the Swap Source and Destination () button in the Source Boundaries section of the contact pair settings.
Small Sliding Contact
In some situations, the relative sliding between the contacting boundaries is small. This is for example often the case for shrink fit simulations, when mounting a component using prestressed bolts, or for partial decohesion of two components. The sliding distance can be considered as small if it is significantly less than the length of a mesh element edge.
In such cases, it is possible to simplify the problem by selecting the Mapping Method to be Initial Configuration in the Contact Pair node. With this setting, a material point on the destination boundary will see the same material point on the source boundary throughout the entire simulation, that is, the mapping is constant. This setting will make the contact analysis run faster and convergence to be more stable.
The analysis is geometrically nonlinear also when using this option, and the contact region can still have arbitrarily large displacements and rotations.
Friction can be modeled. Even though there is no sliding in a geometrical sense, the difference in tangential displacement is computed.
You cannot mix contact pairs with the two different types of Mapping Method within the same Contact node.