COMSOL 6.2 - Setting Up a Contact Problem

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:

•

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 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 when the action is used. The geometric gap distance is a variable set up by the contact pair, which also define operators for mapping variables or expressions between the selected boundaries.

•

Use the default node or add new 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, Slip Velocity, Adhesion, Decohesion, and Wear nodes.

•

Contact Analysis Theory.

•

Identity and Contact Pairs in the COMSOL Multiphysics Reference Manual.

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 is made under Definitions, and can be shared between several physics interfaces. This part of the contact problem defines the geometric properties of the contact, such as search and mapping operations between the selected boundaries. 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. For the default node, this requirement can be removed by selecting .

Including Friction

In real life, there is always some friction between contacting objects, but this is sometimes ignored when setting up the mechanical contact problem. 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 modeling wear.

•

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.

In some cases, such as when a brake pad slides along a brake disc, the size and orientation of the slip velocity is known. You can then employ a simplified form of friction modeling by assuming the tangential contact to always be in a slip state, which simplifies the computation of the friction forces. This is done using the Slip Velocity node. This is particularly useful for wear modeling.

Including 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 model. 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.

Including Wear

It is possible to model adhesive or abrasive wear of the material when the contacting boundaries are sliding along each other. The removal of material from the domain adjacent to the contact boundary can be modeled using three, fundamentally different, approaches.

For the Solid Mechanics and the Multibody Dynamics interfaces, the most general approach relies on the deformed geometry concept, where material is actually removed by using an adaptive mesh technique. In the second, simplified, approach wear is incorporated as an offset in the contact condition. This approach is computationally less expensive, and is suitable as long as only small amounts of material are removed, and wear does not change the orientation of the normal to the boundary significantly. In the Shell and Membrane interfaces the structural domain is represented by only a meshed surface. Therefore, a different, more suitable approach is used, in which the thickness variable and the midsurface offset to the meshed boundary are modified.

Computing the amount of wear involves solving a rate equation, hence, it is only possible to compute wear in time-dependent studies. The wear rate is typically a function of the contact pressure and the relative slip velocity between the contacting boundaries.


	The Wear subnode is not available in the Layered Shell interface.

Selecting the Contact method

In COMSOL Multiphysics, there are three classes of methods available for solving contact problems: the penalty method, the augmented Lagrangian method, and the Nitsche method. For all methods, the contact pair is asymmetric, that is, the destination contact boundary is constrained not to penetrate the source boundary, but not vice versa. However, it is possible to set up a symmetric formulation for the contact problem by selecting the same boundaries as source and destination.

Penalty Method

The default penalty method is rather simple and robust method to introduce the contact conditions. 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. However, the penalty method only enforces the contact conditions approximately. The contact forces computed are thus less accurate than when using, for example, the augmented Lagrangian method, and there is always some overclosure between the contacting surfaces. For stick friction, there is also an “elastic” deformation due to the penalization of the constraint.

When using the penalty method, there is always a tradeoff between accuracy and stability. While a large penalty factor will reduce unphysical 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.

Augmented Lagrangian Method

The augmented Lagrangian method provides better accuracy, but at a higher computational cost, and is often less stable from a convergence point of view. All contact conditions are enforced in a weak or integral sense, and thus evaluated in the integration points on the destination boundary. For normal contact, it is thus possible for a node to have a small penetration into the source boundary, even for a well converged solution. Both, the contact pressure and the friction forces are added as extra degrees of freedom to enforce the contact constraints.

When using the augmented Lagrangian method, it is possible to choose between a segregated and a coupled solution method. The segregated solution method sets up special type of segregated solver sequence, where the extra degrees of freedom related to contact are updated in a separate segregated solver step. As its name implies, there is no such need when using the coupled solution method, and you can more freely set up the solver sequence. This less restrictive solver requirement can be particularly useful for multiphysics problems where the penalty method does not provide sufficient accuracy.

Nitsche Method

The Nitsche method for contact is an extension of the general method suggested by J. Nitsche in 1971 to weakly impose Dirichlet conditions. Conceptually, it can be viewed as an enhancement of the penalty method where the surface traction of the adjacent domains is used to improve the accuracy of the contact condition. Also, as for the penalty method, it has the advantage that no special solver is required, which makes it easier to set up multiphysics problems and time-dependent studies.

The Nitsche method is intended as an alternative to the augmented Lagrangian method for problems where the penalty method lacks sufficient accuracy. Relevant examples where this might be the case includes:

•

Large deformation problems with hyperelasticity

•

Self-contact

•

Problems where the structural stiffness of the global system is of importance

For the first two problems in particular, the accuracy and stability can be further improved by increasing the quadrature order for the contact equations, see also Quadrature Settings. Hence, the Nitsche method uses a higher quadrature order by default than the other contact methods.

COMSOL Multiphysics supports three different formulations of the Nitsche method:

•

Symmetric

•

Skew-symmetric

•

Incomplete

The default incomplete formulation is recommended for the majority of cases and provides a good tradeoff between performance and stability. In cases where the default formulation fails, the skew-symmetric formulation can be an alternative, but it includes additional equations that are expensive to evaluate that can increase the solution time.


	The Nitsche method is available in the Solid Mechanics and Multibody Dynamics interfaces.

Dynamic Methods

Both the penalty and the augmented Lagrangian methods are additionally available in a specialized formulation intended for dynamic contact problems. Both of these are based on a viscous formulation that for the normal contact constrains the rate of the gap to be zero, rather than the gap. Since the formulations are viscous, the duration of the contact should be small, otherwise the overclosure will eventually grow and violate the nonpenetration condition. This is especially the case for the dynamic penalty method, where the gap rate is only approximately zero.

Contact Detection

The contact search is made only toward one side of the source and destination boundaries, determined by the positive direction of the contact normal of the selected boundary. For contact to be detected, this means that the source and destination contact normals must point toward each other. Generally, the contact normal coincides with the geometry normal that is determined by the direction of the boundary. However, there are situations where this is not the case, or where the node can control the sign of the contact normal. Some common situations are summarized in the following:

•

If the contact boundary is on the exterior of a domain, then the geometry normal always point 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, you can select whether the contact should occur on the top side or bottom side. The ‘top’ and ‘bottom’ sides are defined by the orientation of the physics interface normal, which may differ from the geometry normal. 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 actual normal vector used in the contact search algorithm can be visualized by plotting <pair_tag>.n<coord_label>. For example, the variable p1.nx gives the x-component of the spatial normal used by contact pair p1. Plotting the contact normal vector can be useful to verify that the source and destination normals point toward each other.

Visualizing 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.

Contact Between Physics Interfaces

Contact can seamlessly be modeled between Solid Mechanics, Shell, and Membrane interfaces. Equation are only added to nodes that have an applicable destination boundary, that is, a destination boundary that intersects with the selection of the physics interface. Properties such as contact surface offset can, however, be considered as long as either a source or a destination boundary is applicable in the node. Shell and Membrane offsets are automatically considered on both source and destination boundaries.

Source Selection Outside Physics Interfaces

In most cases, 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 a physics interface with a node, the gap is computed using only the current location of its mesh, ignoring any physical properties that may exist there. In this case, the node has no control of the contact normal used by the source boundary. Care must therefore be taken to ensure that the contact normal of the source and destination points toward each other for the contact detection to work.

There are two main scenarios where you may want to use a source selection that is 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