The Contact Model node adds equations to implement the contact condition. It also defines the contact pressure used to enforce the normal contact constraint, such that boundaries in contact may not penetrate each other. The penalty method is always used to implement the contact condition for General Contact.

The penalty factor pn defines the magnitude of the contact pressure for a given gap distance. It is defined as

where fp is a multiplier that can be used to tune the value of the penalty factor. The characteristic stiffness k is defined from a local penalty stiffness estimate kcnt. For each destination boundary, kcnt is defined from properties of the adjacent domain.

The definition of kcnt is controlled by the Penalty stiffness estimation setting. Most common is to use From material stiffness for which kcnt is defined from the equivalent stiffness Eequ of the adjacent domain material, if available, as

where h is the characteristic size of the adjacent domain mesh element.

For transient study steps it is also possible to use From mass. Here, kcnt is defined from the density ρ of the domain material and the current time step Δt of the solver:

Select how to define the Penalty factor multiplier — Automatic; Automatic, soft; or Manual tuning. For Manual tuning enter a dimensionless value for fp.

Select the type of Penalty function — Ramp or Smooth ramp. A smooth penalty function is often useful for impact problems to achieve a less abrupt transition between contact states.

Select Offset penalty function if you want the contact pressure to be nonzero when the gap is zero. For the Ramp function, enter a value for the Contact pressure at zero gap T0. For the Smooth ramp function, enter the Start location Δstart and the Transition zone size Δsize of the function.

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

Select the Integration order — From parent, From displacement field, From displacement field, reduced, or User defined.

When From parent is selected, the integration order is defined in the General Contact node. The other settings are described in Quadrature Settings.

Select how to compute the energy dissipated in the General Contact node.

Select how to Store dissipation — From physics interface, Individual contributions, or Off.

Use From physics interface to treat the dissipative processes as specified in the settings of the physics interface; see, for instance, Energy Dissipation in the Solid Mechanics interface.

Use Individual contributions to treat each dissipative process independently. Selecting this option gives a more flexible implementation for problems where dissipation occurs at different time scales, and you want to distinguish each phenomenon separately.

Use Off to ignore the accumulation of dissipative processes.

Select how to define the Characteristic stiffness k — Harmonic mean, Minimum, Destination only or From fallback stiffness.

Enter a value for the Fallback stiffness kfb. The fallback stiffness is used if a definition of kcnt is not available. For example, boundaries adjacent to a Rigid Material will always use kfb.

The state of being in contact or not is used by other features or physics. Since the gap value for the penalty method will never be exactly zero, even when the boundaries are in contact, also a small positive the gap is typically 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 Δcnt.

Physics tab with General Contact selected in the Model Builder tree: