Contact
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.
If friction is to be included in the modeling, add a Friction subnode.
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/).
In order to specify contact conditions, one or more Contact Pair nodes must be available in the Definitions branch.
If you have several interfaces with displacement degrees of freedom in your model, only the last physics interface in the model tree can contain contact physics features since that is the physics interface in which the displacements controls the spatial frame.
When a contact feature is present in your model, all studies are geometrically nonlinear. The Include geometric nonlinearity check box on the study step Settings window is selected and cannot be cleared.
A Contact node will override all previous nodes in the Model Tree sharing the same boundary selections. If you want to add a load (such as the pressure of a surrounding fluid), the best way of doing that is to select a Boundary Load from the Fallback Features of the Contact node. Such a load will then act only on the portions of the boundaries not being in contact.
If an ordinary Boundary Load node is added after the Contact node in the Model Tree, it will contribute to the load on the boundaries, but without taking the contact state into account.
•
Contact Modeling
•
Contact Analysis Theory
Contact Pressure Method
Select the algorithm used for computing the contact in the normal direction, Augmented Lagrangian (default) or Penalty.
Enter a value for Characteristic stiffness Echar. The default is solid.Eequ, the equivalent Young’s modulus as defined by most materials. The characteristic stiffness (stored in a variable named solid.<contact_tag>.E_char) is used in expressions for the default penalty factors for both the Augmented Lagrangian and Penalty methods. It 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:
•
The material is strongly anisotropic. The default value is based on an average in all directions.
•
The material is highly nonlinear. The default value is based on the stiffness at zero strain.
•
The variable solid.Eequ is not defined by the material. This is the case for some user defined materials.
Penalty Factor
If Contact Pressure Method is Augmented Lagrangian, 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.
In the augmented Lagrangian method, the penalty factor controls how “hard” the interface surface is during the iterations, but it does not affect the converged result. You can consider the penalty factor as a spring giving a resisting force if the boundaries in the contact pair have an interference. A larger value gives faster, but less stable, convergence to the state where there is no interference. A too large value can create convergence difficulties, particularly if the interference is large
In the penalty method, the penalty factor is the actual stiffness of a spring inserted between the boundaries in the contact pair.
If you select Preset, you have the choices to select Tuned for as Stability (default) and Speed. If the contact boundaries move towards each other, so that large interferences 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.
If relaxation is used, enter the Initial Relaxation Factor. The default is 0.005. This factor multiplies the penalty factor in the first iteration. Enter Number of iterations with relaxation. 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 interference 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. Edit or use the default Contact pressure penalty factor pn.The default value is min(1e-3*5^niterCMP,1)*solid.<contact_tag>.E_char/solid.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 solid.<contact_tag>.E_char is the characteristic stiffness as defined in the Contact Pressure Method section, and hmin_dst is the minimum element size on the destination.
When Contact Pressure Method is Penalty, enter the Contact pressure penalty factor pn. The default value is solid.<contact_tag>.E_char/solid.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.
Trigger Cutback
This section is only available when Contact Pressure Method is Augmented Lagrangian. Select the Trigger cutback check box to enable additional control over solver cutbacks in Time Dependent study or Stationary study with a Parametric continuation solver. 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 does 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.
In the COMSOL Multiphysics Reference Manual:
•
Time Dependent and Stationary
•
About the Time-Dependent Solver and About the Parametric Solver
Offset and Adjustment
Enter a value or expression for Contact surface 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 Contact surface 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 touch each other in the initial state. The gap is adjusted to zero before any offset is added.
Use the offset properties to adjust initial clearances (negative values) or interference fits (positive values) without having to change the geometry. These properties are also useful for studying the effects of geometrical tolerance when the structure is still modeled using its nominal size.
When combined with Force zero initial gap, the offset will be exact in the sense that it is not affected by mesh irregularities.
The adjustment made by Force zero initial gap does not move any nodes in the mesh. Effectively it adds an extra hidden offset, which compensates for any initial distance between source and destination boundaries.
Offset and Adjustment
Initial Values
This section is only available when Contact Pressure Method is Augmented Lagrangian. Enter an initial value for the Contact pressure Tn.
If not all the contacting parts are fully constrained, it is important to supply a value here in order to avoid singular problems.
Speed up the convergence by supplying a guess of the correct order of magnitude of the contact pressure.
Discretization
This section is only available when Contact Pressure Method is Augmented Lagrangian. To display this section, click the Show button () and select Discretization. Select a shape-function order for Contact pressure — Linear (the default), Quadratic, Cubic, Quartic, or (in 2D) Quintic. This setting should usually not be changed. Selecting anything else than Linear requires that the solver sequence is modified manually because the lumped solver is then no longer optimal for the contact pressure update.
Advanced
To display this section, click the Show button () and select Advanced Physics Options.
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 printout about the changes in the solver log window. Doing this will add extra dependent variables used for tracking the contact state on the destination boundaries.
If you have more than one contact pair selected in the Contact node, and the augmented Lagrangian method is used, the check box Group contact variables in solver per pair will be shown. When selected, a new Lumped Step will be generated in the segregated solver for each contact pair. This will not affect the solution, but will give more granular output in the convergence plots.
Select Store energy variables to get access to
Location in User Interface
Context Menus
 Solid Mechanics>Pairs>Contact
 Multibody Dynamics>Pairs>Contact
Ribbon
Physics tab with Solid Mechanics or Multibody Dynamics selected:
Pairs>Contact