In the Contact node, you define the mechanical and numerical properties for a set of contact pairs in a contact analysis. Use it for modeling structural contact and multiphysics contact. In the latter case, you will also need to add corresponding pair conditions in the other participating physics interfaces.

In the contact pair, the destination side selection must be part of the physics interface in which you add the Contact node. The source side selection can be any kind of meshed object, but if it is part of the current physics interface, more options are made available.

If friction is to be included in the modeling, add a Friction subnode. You can also model perfect bonding and debonding of the contact pair using the Adhesion and Decohesion subnodes.

Do not select the same contact pair in more than one Contact node. Doing so may produce error messages or unpredictable results.

The Contact node is only available with some COMSOL products (see http://www.comsol.com/products/specifications/).

For Contact surface, destination and Contact surface, source, select Top or Bottom. The top side is the one with an outward pointing normal vector.

The setting for the source side is not available if Source external to current physics is selected in the Contact Method section.

Select the algorithm used for computing the contact, Penalty (default) or Augmented Lagrangian. The augmented Lagrangian method is in general more accurate than the penalty method, but also more expensive in terms of computer resources.

If the source side of the contact pair is not part of the current physics interface, select Source external to current physics. When selected, only the location of the mesh on the source side is taken into account when evaluating the contact.

Enter a value for Characteristic stiffness Echar. The default is <phys>.Eequ, the equivalent Young’s modulus as defined by most material models. The characteristic stiffness (stored in a variable named <phys>.<contact_tag>.E_char) is used in expressions for the default penalty factors for both the penalty and the augmented Lagrangian methods. The characteristic stiffness should be representative for the stiffness of the destination domain material in a direction normal to the boundary. You may for example need to adjust the default value in for the following cases:

Select the type of Penalty factor control — Automatic or User defined. For User defined, enter the Contact pressure penalty factor pn. The default value is <phys>.<contact_tag>.E_char/<phys>.hmin_dst.

Click to select Offset penalty function if you want the contact pressure to be nonzero when the gap is zero. In that case, also enter a value for the Contact pressure at zero gap T0. Through this option, you can to some extent compensate for the overclosure that is inherent to the penalty method if you know an approximate value of the expected contact pressure.

Select the type of Penalty factor control — Preset (default), Manual tuning, or User defined. The settings give access to an increasing level of detailed control of the penalty factor.

If you select Preset, you have the options to select Tuned for to be Stability (default) or Speed. If the contact boundaries move toward each other, so that large overclosures can be expected in the initial iterations, then is Stability is the better choice. In many models, where the contact state does not change much, using Speed gives significant performance improvements.

The Penalty factor control selection Manual tuning gives you access to a number of detailed settings for the penalty factor.

Enter a Penalty factor multiplier. The default value is 1. Increasing this factor gives a higher penalty factor. From Use relaxation, select Always (default), Never, or Conditional. When using relaxation, the penalty factor is decreased during the first iterations in each parameter or time step. The purpose is to avoid large residuals in the case of a large initial overclosure between the contacting boundaries.

If relaxation is used, enter the Initial Relaxation Factor, ri. The default is 0.005. This factor multiplies the penalty factor in the first iteration. Enter Number of iterations with relaxation, Nr. The default value is 4. The penalty factor is gradually increased up to its full value, which is used in the iteration after the one where the specified number of iterations with relaxation have been reached.

If Use relaxation is set to Conditional, enter a Suppression criterion. The default is 0, which means that the relaxation is used for all parameter or time steps. This is a Boolean expression which, when fulfilled, suppresses the relaxation. If you, for example, know that your problem needs relaxation only during the initial phase of the solution, you could enter en expression like load_parameter>0.1. It is also possible to use expressions based on the solution, for example abs(solid.cnt1.gap)<0.05*h. This expression is true when the gap or overclosure is small compared to the mesh size. It could be taken as an indication that the contact problem is almost converged, and thus not in need of any relaxation of the penalty factor.

Using the Penalty factor control selection User defined gives you the possibility to enter an explicit expression for penalty factor. Enter the Contact pressure penalty factor pn.The default value is (min(1e-3*(5^niterCMP,1))*<phys>.<contact_tag>.E_char)/<phys>.hmin_dst. The default value causes the penalty factor to be increased during the iterations and takes material stiffness and element size at the contact surface into account. The variable <phys>.<contact_tag>.E_char contains the value given as Characteristic stiffness, and hmin_dst is the minimum element size on the destination selection.

This section is only available when Formulation is Augmented Lagrangian. Select the Trigger cutback check box to enable additional control over solver cutbacks in a time-dependent study or a stationary study with an auxiliary sweep. Enter a logical expression for Cutback criterion. When this expression evaluates to a nonzero value, the iterations are immediately terminated, and the solver tries to use a smaller value of the time or parameter. You can use this setting to avoid that the solver spends many iterations trying to recover from an unphysical state. As an example, if you know that the destination boundary is confined so that it will not move more than 1 mm anywhere, an entry like solid.disp > 5[mm] can be useful, since it is unlikely that a displacement of this size should appear during a successful iteration history.

Enter a value or expression for Offset from geometric destination surface doffset,d. The offset is subtracted from the gap in the normal direction of the destination surface.

Enter a value or expression for Offset from geometric source surface doffset,s. The offset is subtracted from the gap in the normal direction of the source surface.

Select Force zero initial gap to compensate for any difference caused by irregularities in geometry or mesh when the two contacting boundaries should exactly coincide in the initial state. Gaps smaller than the tolerance Δgap are adjusted to be zero before any offset is added. By default Δgap is set to Inf, meaning that all gaps detected are adjusted to be zero.

This section is only available when Formulation is Augmented Lagrangian. In the augmented Lagrangian method, the contact pressure is introduced as an extra dependent variable on the destination boundaries. Enter a value for Contact pressure Tn to supply an initial value for the contact pressure.

To display this section, click the Show More Options button () and select Advanced Physics Options in the Show More Options dialog box.

This section is only available when Formulation is Augmented Lagrangian. In the augmented Lagrangian method, the contact pressure is introduced as an extra dependent variable on the destination boundaries. You can modify the discretization order of this field. The main reason to do so is when you use a higher order for the displacement shape functions than the default quadratic. In that case, a consistent choice of discretization order for the contact pressure is one order lower than what is used for the displacements.

To change the discretization, select a shape-function order — Linear, Quadratic, Cubic, Quartic, or (in 2D) Quintic. The lumped solver is only optimal when the shape-function order is Linear, otherwise use a standard segregated step instead.

To display this section, click the Show More Options button () and select Advanced Physics Options in the Show More Options dialog box.

When analyzing a multiphysics contact problem, the state of being in contact or not will be passed from the contact analysis in the structural mechanics interface to other participating physics interfaces. For numerical reasons, the gap value will however not be exactly zero, even when the boundaries are in contact. A certain small positive value of the gap will thus be considered as being in contact. The default Multiphysics contact tolerance is Automatic. If you want to explicitly specify the limit of the gap considered as being in contact, select Manual, and enter the Contact tolerance Δcontact.

Select Add contact status to solver log to get printouts about the change in the contact state in the solver log window. Doing so will add internal dependent variables used for tracking the contact state on the destination boundaries.

Physics tab with Solid Mechanics, Layered Shell, Shell, Membrane, or Multibody Dynamics selected: