Setting up a contact problem
Mechanical contact can be modeled in the Solid Mechanics and Multibody Dynamics interfaces. To model a mechanical contact problem, you must do the following:
•
Add Contact Pair nodes under Definitions. A contact pair consists of two sets of boundaries, which are called the source and destination boundaries.
•
Add Contact nodes in the physics interface. In the Contact node, you select the contact pairs to be used, and provide the settings for the physical and numerical properties of the contact model.
•
In the finalization step of the geometry sequence, you should normally have Action set to Form an assembly. If Form a union is used, then the contacting boundaries must be geometrically separated in the initial configuration.
•
Select a suitable study type. You can analyze contact using a Stationary or Time Dependent study step.
•
Documentation of the Contact, Friction and Adhesion nodes.
•
Contact Analysis Theory.
•
Identity and Contact Pairs in the COMSOL Multiphysics Reference Manual.
•
Time-Dependent Contact Analysis.
In a multiphysics analysis, a contact problem can also incorporate for example changes in the heat flux or electric current through the contacting boundaries. You will then also need to add corresponding features in the other participating interfaces, like a Thermal Contact node in the Heat Transfer in Solids interface. The contact state and contact pressure used in other physics interfaces is always supplied by the structural mechanics interface.
The fact that you add a Contact node to your model will make all study steps geometrically nonlinear.
Including Friction
In real life, there is always some friction between contacting objects, but this is often ignored. There are several reasons to do this simplification:
•
In many cases, only the normal forces are significant for the general force distribution in the structure, while the frictional forces only cause a minor local effect.
•
The values of the friction coefficients are difficult to obtain, and unless the structure is assembled under well controlled conditions, the magnitude of the friction can vary a lot.
•
Adding friction to a contact problem will often increase the computation time significantly, or even cause convergence problems.
There are a number of situations when friction modeling cannot be avoided. Some of them are:
•
When a significant portion of the load is carried by shear stresses in the contact boundaries.
•
When a tangential force is necessary to maintain stability and avoid rigid body motions. In many cases, it is however possible to replace the friction by a suitable constraint instead, as long as there are no resultant forces being resisted by such a constraint.
•
When the frictional dissipation is an important component of a dynamics problem, or when it is needed as a heat source in a thermal analysis.
Adhesion and Decohesion
You can also specify that the contacting boundaries stick to each other so that they will not separate or slide. The onset of adhesion, when the boundaries become permanently attached to each other, can be based on several criteria:
•
When a certain contact pressure is exceeded.
•
When the gap distance between the contact boundaries is smaller than a certain value.
•
When a user specified logical expression is fulfilled. This can for example be used if an adhesive cures when a certain temperature is exceeded.
•
From the start of the analysis. This case is particularly interesting if you are interested in modeling the tearing of a thin glue layer by decohesion.
If adhesion is active between the contact boundaries, it is possible to break the bond by adding a decohesion rule. You can choose between several different decohesion laws.
Selecting the Contact Algorithm
In COMSOL Multiphysics, there are two possible methods for solving contact problems: the augmented Lagrangian method and the penalty method.
The default augmented Lagrangian method provides better accuracy, but at a higher computational cost. It requires additional degrees of freedom, and is less stable from the convergence point of view. This method ensures that there will not be any penetration between the contacting objects in a well converged solution. The contact pressure and friction forces are added as degrees of freedom. The contact pair is asymmetric (that is, it is a source/destination pair). The destination contact domain is constrained not to penetrate the source domain, but not vice versa. The contact condition is evaluated in the integration points on the destination boundary. It is thus possible for a node to have a small penetration into the source boundary, even in a converged state.
In comparison, the penalty method is rather simple and robust. Roughly speaking, it is based on inserting a stiff spring, active only in compression, between the contacting boundaries. In addition to the robustness, it has the advantage that no special solver is required, which makes it easier to set up multiphysics problems and time-dependent studies.
The penalty method must be used when modeling adhesion.
You can select the method used for computing the normal direction pressure and the friction forces independently.