In the Interior Contact node, you define contact conditions for a set of interior boundaries in a solid model. This contact formulation provides a simplified setup that does not require the addition of contact pairs. It is limited so small-scale sliding between the contact boundaries.

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

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

When Augmented Lagrangian is selected, it is also possible to choose Solution method —Segregated (default) or Fully coupled. This setting affects how the default solver suggestion is set up when generating a new solver sequence, as well as some variable definitions and equations.

The Nitsche method can conceptually be seen as an enhancement of the penalty method where the surface traction of the adjacent domains is utilized to improve accuracy. For Interior Contact, the only available Formulation is Incomplete.

Select the type of Penalty factor control — Automatic; Automatic, soft; Manual tuning; Nonlinear; or User defined.

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, and are available when Solution method is set to Segregated.

If you select Preset, you have the options to select Tuned for to be Stability (default), Speed, or Bending. If the contact boundaries move toward each other, so that large overclosures can be expected in the initial outer iterations, then Stability is the better choice since it relaxes the penalty factor during the first iterations. In many models, where the contact state does not change much, using Speed gives significant performance improvements. The Bending option provides a low penalty factor equal to the one used for the first iterations when using Stability. This option thus provides a conservative algorithm that can be particularly useful for problems dominated by bending. However, it might require many iterations to reach convergence.

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 fp. The default value is 1. From Use relaxation, select Always (default), Never, or Conditional. When using relaxation, the penalty factor is decreased during the first outer 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 outer 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 outer 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, enter an expression like load_parameter>0.1. It is also possible to use expressions based on the solution, for example abs(solid.icnt1.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 is (min(1e-3*(5^niterCMP,1))*<phys>.<contact_tag>.E_char)/<phys>.<contact_tag>.hmin_dst. The default value causes the penalty factor to be increased during the outer iterations and takes material stiffness and element size at the contact surface into account. The variable E_char contains the value given as characteristic stiffness, and hmin is the minimum element size on the selected boundaries.

Select the type of Penalty factor control — Automatic (default), Manual tuning, or User defined.

Enter a value or an expression for Offset doffset. The offset is subtracted from the gap in the normal direction.

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.

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 shape function type and order of this field. The default is to always use a linear shape function order for the contact pressure, but using a higher order can improve the accuracy of the contact condition. A value up to the discretization order of the displacement field is allowed. This setting also affects the shape function for dependent variables added by any subnode added to the Contact node.

To change the discretization, select Shape function type — Lagrange or Nodal serendipity.

The lumped solver used for the segregated augmented Lagrangian method is only optimal when the shape function order is Linear; otherwise, use a standard segregated step instead. The proper solver sequence is set up when adding a new default solver.

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

Typically, the expressions in the contact weak equations include discontinuous functions. It is sometimes preferable to use a high integration order to improve the accuracy of the numerical integration of such expressions. By default, the numerical integration of the contact weak equations is twice the shape function order of the displacement field. Clear the Use automatic quadrature settings checkbox to specify a custom order. When the checkbox is cleared, enter an integer value between 0 and 41 in the Integration order field. This setting also affects the integration order for any subnode added to the Contact node.

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

Enter a 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:

Physics tab with Solid Mechanics or Solid Mechanics, Explicit Dynamics selected: