Setting Up a Contact Problem

Mechanical contact can be modeled between boundaries in the Solid Mechanics, Multibody Dynamics, Shell, Layered Shell, and Membrane interfaces. You can model contact not only within a single physics interface, but also between two physics interfaces, or even between a physics interface and any boundary having a mesh.

To model a mechanical contact problem, you must do the following fundamental steps:

•

Add nodes under . A contact pair consists of two sets of boundaries, which are called the source and destination boundaries. Contact pairs can also be added automatically, based on boundary adjacency. The gap distance is a property of the contact pair.

•

In the finalization step of the geometry sequence, you should normally have set to . If is used, then the contacting boundaries must be geometrically separated in the initial configuration.

•

Add nodes in the physics interface. In the node, you select the contact pairs to be used, and provide the settings for the physical and numerical properties of the contact model.

•

If relevant, add , , or subnodes to .

•

Select a suitable study type. You can analyze contact using the following types of study steps:

Stationary; commonly using an auxiliary sweep.

Bolt Pretension

Time Dependent

Any type of prestressed analysis. In this case, the full contact problem is solved in the preload step, and in the subsequent perturbation step the contact state is considered as fixed.

•

Documentation of the Contact, Friction, Adhesion and Decohesion 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 node in the Heat Transfer in Solids interface. The contact state and contact pressure used by other physics interfaces are always supplied by the structural mechanics interface.


	Because of the multiphysics capabilities, the setup of a contact problem is split into two parts. The definition of the contact pair (essentially its geometry) is made under Definitions, and can be shared between several physics interfaces. The physics related definitions of the contact properties are then made in the respective physics interfaces.

The fact that you add a node to your model will automatically 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 minor local effects.

•

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. If there is a large degree in uncertainty in the input data, it can be argued that the inclusion of friction does not add much to the quality of the results.

•

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 tractions acting on the contact boundaries.

•

When a tangential force is necessary to maintain stability and to avoid rigid body motions. In many cases, it is however possible to replace the friction by a suitable boundary condition 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.


	Friction is not available with the Layered Shell interface.

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 useful if you are interested in modeling the subsequent 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 models.

Adhesion and friction can be combined, but during the time that two boundaries are bonded to each other through adhesion, any settings for friction are ignored.


	Adhesion and Decohesion is not available with the Layered Shell interface.

Selecting the Contact Algorithm

In COMSOL Multiphysics, there are two possible methods for solving contact problems: the penalty method and the augmented Lagrangian method.

Penalty Method

The default penalty method is rather simple and robust method to introduce the contact condition. Roughly speaking, it is based on inserting a stiff distributed 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 contact forces computed by the penalty method are less accurate than when using the augmented Lagrangian method, and there is always some overclosure between the contacting surfaces.

When using the penalty method, there is always a tradeoff between accuracy and stability. While a large penalty factor will reduce nonphysical overclosures, the problem may become ill-conditioned and unstable if it is too large. It might therefore be beneficial to accept some penetration between the contacting objects. Note, however, that if the penalty factor is too small, the contact condition may be violated.

Adhesion and Decohesion is only available together with the penalty method.

Augmented Lagrangian Method

The 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 extra degrees of freedom. The contact pair is asymmetric (that is, it is a source/destination pair). The destination contact boundary is constrained not to penetrate the source boundary, 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.

When using the augmented Lagrangian method a special type of segregated solver sequence must be used, where the extra degrees of freedom are updated in a separate segregated solver step.

Source Selection Outside Physics Interface

In most cases, the elements on both the source and destination boundaries belong to the same physics interface. The only strict rule, however, is that the destination side belongs to the physics interface in which the node resides. The source side only needs to have a mesh, and can optionally have one or more physics interfaces attached to it.

If the source boundary is not part of the current physics interface, the gap is computed using only the current location of its mesh, ignoring any physical properties that may exist there.

There three main scenarios where you may want to use a source selection not in the current physics interface:

Fixed Rigid Wall

If one side of a contact pair can be considered as rigid and fixed in space, then it is sufficient to add a meshed boundary at that location without any physics.

Moving Rigid Wall

Different Physics Interfaces

In cases where you want to model contact between, for example, a 3D solid modeled in the Solid Mechanics interface, and a boundary modeled in the Shell interface, you can use this technique. In principle, you can put the node in either of the physics interfaces, but it should not be used in both.

In practice, however, you will typically want to place the node in the Shell interface, if that is one of the participating interfaces. The reason is that this is the only way to account for the actual shell thickness and possible offset in a contact analysis. When the source selection does not belong to the physics interface, only the location of the mesh in known when setting up the contact equations.

Contact Direction

The contact conditions are considered on only one side of the destination and source boundaries. In most cases, the positive direction of the normal to the boundary defines the direction on which contact can occur.

•

If the source boundary is on the exterior of a domain, then the geometry normal always points outward from the domain. This is the most common case, and then no other considerations are needed.

•

In some cases, like fluid-structure interaction, there may be a domain with a moving mesh between the two contacting objects. The source and destination boundaries will then, in the geometrical sense, be interior boundaries. In this case, the physics interface (Solid Mechanics or Multibody Dynamics) defines a normal vector which is pointing outward from the boundaries that are external to the physics interface. Thus, this case is also handled automatically.

•

When a boundary without an adjacent domain is selected, you need to be careful so that the normal is pointing in the intended direction.

•

When using the Shell, Layered Shell or Membrane interfaces, contact can potentially occur on both sides of the boundary. In a single node, you can only model contact on one side. In the section of the settings for the node, you can select whether the contact should occur on the top side (positive normal direction) or bottom side. In these interfaces, the orientation of the physics normal is controlled by the Boundary System that is attached to each boundary through the material models. The normal direction can be reversed using the settings in the node. The ‘top’ and ‘bottom’ sides are defined by the orientation of the physics interface normal, which may thus differ from the geometry normal. If a Shell, Layered Shell or Membrane interfaces is an external source to a node, the geometry normal of the boundary should point at the destination boundary


	When using the Layered Shell interface, it is recommended to set up the contact problem so that the contact surface is the ‘top’ side of the shell. Furthermore, the preferred position of the layered material ‘Upside on boundary’.

Determining the Orientation of Boundaries

In 2D, a boundary is represented by a line. If you follow the line from its start point to its endpoint, the positive normal points to the left. The line orientations can be visualized by selecting the check box in the appropriate node under .

In 3D, the rules for the orientation of a boundary are more complicated. In general, you have to visualize the normals, in order to check its orientation. This can be done in different ways:

•

For a mesh without physics, you will need to use the general result presentation tools. Follow these steps:

Run for an arbitrary study in order to create data for result presentation.

Add a under .

Add an plot to the new plot group.

In the (

) dialog, select the geometry normal.

•

When working with the Shell or Membrane interfaces, select in the settings for the interface. You will then see the physics normals plotted if you select a material model like in the Model Builder.