The Advanced category provides the following properties.
Formulation options allow you to specify which algorithm the software uses for a particular Contact pair computation.
Property options include:
|
Property |
Description |
MAPDL |
| This is the default setting. For this setting, the application selects the Pure Penalty property for contact between two rigid bodies and the Augmented Lagrange property for all other contact situations. | - | |
| Basic contact formulation based on Penalty method. |
KEYOPT(2) = 1 | |
| Also a penalty-based method. Compared to the Pure Penalty method, this method usually leads to better conditioning and is less sensitive to the magnitude of the contact stiffness coefficient. However, in some analyses, the Augmented Lagrange method may require additional iterations, especially if the deformed mesh becomes too distorted. |
KEYOPT(2) = 0 | |
| Available for and for
contact
Types. Multipoint Constraint equations are created
internally during the Mechanical APDL application solve to tie the bodies
together. This can be helpful if truly linear contact is desired or to
handle the nonzero mode issue for free vibration that can occur if a
penalty function is used. Note that contact based results (such as
pressure) will be zero. Note: When modeling Shell-Solid assemblies with the MPC contact Formulation, the contact surface/edge must be on the shell side and the target surface must be on the solid side. However, you can override this requirement to support certain special cases, such as acoustics. See the Modeling a Shell-Solid Assembly section of the Mechanical APDL Contact Technology Guide for additional information. |
KEYOPT(2) = 2 | |
| Enforces zero penetration when contact is closed making use of a Lagrange multiplier on the normal direction and a penalty method in the tangential direction. Normal Stiffness is not applicable for this setting. Normal Lagrange adds contact traction to the model as additional degrees of freedom and requires additional iterations to stabilize contact conditions. It often increases the computational cost compared to the Augmented Lagrange setting. The Iterative setting (under Solver Type) cannot be used with this method. |
KEYOPT(2) = 3 | |
| Available for Type only. This formulation works by "stitching" the contact topologies together using massless linear Beam Elements. | - |
For additional Mechanical APDL specific information, see KEYOPT(2) in the Mechanical APDL Contact Technology Guide.
Note: Cases involving large gaps and faces bonded together can result in fictitious moments being transmitted across a boundary.
The Small Sliding property displays and activates an assumption of relatively-small sliding (less than 20% of the contact length during the analysis). If small sliding is known to occur, such as when you have bonded contact, this feature can make your solution more efficient and robust.
Property options include:

|
Property |
Description |
|
|
This is the default setting. The application determines whether small sliding logic is enabled. |
|
|
Enable small sliding. |
|
|
Disable small sliding |
For additional information, see the Selecting a Sliding Behavior topic in the Mechanical APDL Contact Technology Guide.
Detection Method enables you to choose the location of contact detection used in the analysis in order to obtain a good convergence. It is applicable to 3D face-face contacts and 2D edge-edge contacts.
Property options include:

|
Property |
Description |
|
|
This is the default setting. The application uses Gauss integration points (On Gauss Point) when the formulation is set to Pure Penalty and Augmented Lagrange. It uses nodal point (Nodal-Normal to Target) for MPC and Normal Lagrange formulations. |
|
|
The contact detection location is at the Gauss integration points. This option is not applicable to contacts with MPC or Normal Lagrange formulation. |
|
|
The contact detection location is on a nodal point where the contact normal is perpendicular to the contact surface. |
|
|
The contact detection location is on a nodal point where the contact normal is perpendicular to the target surface. |
|
|
The contact detection location is at contact nodal points in an overlapping region of the contact and target surfaces (projection-based method). |
For additional Mechanical APDL specific information, see Selecting Location of Contact Detection (specifically, KEYOPT(4) related information) in the Mechanical APDL Contact Technology Guide.
The Penetration Tolerance property enables you to specify the Penetration Tolerance Value or the Penetration Tolerance Factor for a contact when the Formulation property is set to , , or .
Note: The Update Stiffness property must be set to either , , or for the Penetration Tolerance property to be displayed when Formulation is set to .
Property options include:

| Property | Description |
| Program Controlled | This is the default setting. The Penetration Tolerance is calculated by the program. |
| Value | Enter the Penetration Tolerance directly. This entry is a length measurement (foot, meter, etc.). Only non-zero positive values are valid. |
| Factor | Enter the Penetration Tolerance directly. This entry must be equal to or greater than zero but must also be less than 1.0. This entry has no unit. |
Penetration Tolerance Value
The Penetration Tolerance Value property displays when Penetration Tolerance is set to . You enter a Value.
Penetration Tolerance Factor
The Penetration Tolerance Factor property displays when Penetration Tolerance is set to . You enter a Factor.
Note: When viewing the Connections Worksheet, a displays as a negative number and a displays as a positive number.
For additional information, see the Determining Contact Stiffness and Allowable Penetration, specifically Using FKN and FTOLN, section of the Mechanical APDL Contact Technology Guide (Surface-to-Surface Contact).
The Elastic Slip Tolerance property enables you to set the allowable elastic slip value for a contact when the Formulation is set to Normal Lagrange or when the contact stiffness is set to update each iteration (Update Stiffness is set to or ).
Note: Elastic Slip Tolerance is not applicable when the contact Type is set to Frictionless or No Separation.
Property options include:

| Property | Description |
| Program Controlled | This is the default setting. The Elastic Slip Tolerance Value is calculated by the application. |
| Value | Enter the Elastic Slip Tolerance Value directly. This entry is a length measurement (foot, meter, etc.). Only non-zero positive values are valid. |
| Factor | Enter the Elastic Slip Tolerance Factor directly. This entry must be equal to or greater than zero but must also be less than 1.0. This entry has no unit. |
Elastic Slip Tolerance Value
The Elastic Slip Tolerance Value property displays when Elastic Slip Tolerance is set to . You enter a Value.
Elastic Slip Tolerance Factor
The Elastic Slip Tolerance Factor property displays when Elastic Slip Tolerance is set to . You enter a Factor.
Note: When viewing the Connections Worksheet, a displays as a negative number and a displays as a positive number.
For additional information, see the Determining Contact Stiffness and Allowable Penetration, specifically Using FKT and SLTO, section of the Mechanical APDL Contact Technology Guide (Surface-to-Surface Contact).
The Constraint Type property controls the type of MPC constraint to be created for bonded contact. This displays only if Formulation property is set to MPC and if either Contact Bodies or Target Bodies are scoped to a surface body. The property includes the following options:

|
Property |
Description |
| Program Controlled |
This is the default setting. Internally this corresponds to the Projected, Displacement Only option for solid-solid contact and Distributed, All Directions option for all other contact types. |
| Projected, Displacement Only |
Constraints are constructed to couple the translational DOFs only. Projected constraint if an intersection is found from the contact normal to the target surface. |
| Projected, Uncoupled U to ROT |
The rotational and displacement constraints will not be coupled together. This option can model situations where the surface body edges line up well and a moment is not created from the physical surface body positions. Thus it is most accurate for the constraints to leave the displacements/rotations uncoupled. This provides an answer which is closer to a matching mesh solution. Using a coupled constraint causes artificial constraints to be added causing an inaccurate solution. |
| Distributed, Normal Only |
Both translational DOFs and rotational DOFs of contact nodes and translational DOFs of target nodes are included in the constraint set in a coupled manner. |
| Distributed, All Directions |
Represents the most common type of surface body contact. Constraints are constructed to couple the translational and rotational DOFs. In most types of surface body contact, an offset will exist. Due to this offset there will be a moment created. To get the correct moment, the rotation/displacement DOF's must be coupled together. If the program cannot detect any contact in the target normal direction, it will then search anywhere inside the pinball for contact. |
| Distributed, Anywhere Inside Pinball |
Constraints are coupled and created anywhere to be found inside the pinball region. Thus the pinball size is important as a larger pinball will result in a larger constraint set. This option is useful when you wish to fully constrain one contact side completely to another. |
For additional information, see the Controlling Degrees of Freedom Used in the MPC Constraint topic in the Modeling Solid-Solid and Shell-Shell Assemblies section of the Mechanical APDL Contact Technology Guide. Also note that the Mechanical APDL entry for the Constraint Type is KEYOPT(5) for element TARGE170.
Defines a contact Normal Stiffness factor. Property options include:
|
Option | Description |
| Program Controlled |
This is the default setting. The Normal Stiffness Factor is calculated by the program. If only Bonded or No Separation contact exists, the value is set to 10. If any other type of contact exists, all the program controlled regions (including Bonded or No Separation) will use the Mechanical APDL application default (Real Constant FKN). |
| Manual |
The Normal Stiffness Factor is input directly by the user. |
This property appears when the Normal Stiffness is set to Manual. It enables you to input the Normal Stiffness Factor. Only non-zero positive values are allowed. The usual factor range is from 0.01-10, with the default selected programmatically. A smaller value provides for easier convergence but with more penetration. The default value is appropriate for bulk deformation. If bending deformation dominates, use a smaller value (0.01-0.1).
For additional Mechanical APDL specific information, see the
Determining Contact Stiffness and Allowable Penetration section of the Mechanical APDL Contact Technology Guide (Surface-to-Surface Contact).
Using FKN and FTOLN section of the Mechanical APDL Contact Technology Guide (Surface-to-Surface Contact).
enables you to specify if the program should update (change) the contact stiffness during the solution.
If you choose any of these stiffness update settings, the program will modify the stiffness (raise/lower/leave unchanged) based on the physics of the model (that is, the underlying element stress and penetration). This choice is displayed only if you set the Formulation to Augmented Lagrange or Pure Penalty, the two formulations where contact stiffness is applicable.
An advantage of choosing either of the program stiffness update settings is that stiffness is automatically determined that allows both convergence and minimal penetration. Also, if this setting is used, problems may converge in a Newton-Raphson sense, that would not otherwise.
You can use a Result Tracker to monitor a changing contact stiffness throughout the solution.
Property options include:

|
Property |
Description |
| Program Controlled |
(Default as set in Tools>Options). Internally set based on the following criteria: set the Update Stiffness property to for contacts between two rigid bodies and to for all other cases. |
| Never | This is the default setting. Turns off the program's automatic Update Stiffness feature. |
|
Sets the program to update stiffness at the end of each equilibrium iteration. This choice is recommended if you are unsure of a to use in order to obtain good results. | |
|
Sets the program to update stiffness at the end of each equilibrium iteration, but compared to the , this option allows for a more aggressive changing of the value range. |
A contact you define may initially have a near open status due to small gaps between the element meshes or between the integration points of the contact and target elements. The contact will not get detected during the analysis and can cause a rigid body motion of the bodies defined in the contact. The stabilization damping factor provides a certain resistance to damp the relative motion between the contacting surfaces and prevents rigid body motion. This contact damping factor is applied in the contact normal direction and it is valid only for frictionless, rough and frictional contacts. The damping is applied to each load step where the contact status is open. The value of the stabilization damping factor should be large enough to prevent rigid body motion but small enough to ensure a solution. A value of 1 is usually appropriate.
Property options include:
|
Property |
Description |
Mechanical APDL |
|---|---|---|
|
Stabilization Damping Factor |
If this factor is 0 (default), the damping is activated only in the first load step (KEYOPT(15) = 0, the default). If its value is greater than 0, the damping is activated for all load steps (KEYOPT(15) = 2). |
KEYOPT(15) = 2. Damping is activated for all load steps. |
Controls the thermal contact conductance value used in a thermal contact simulation.
Property options include:
|
Property |
Description |
| Program Controlled | This is the default setting. The program will calculate the value for the thermal contact conductance. The value will be set to a sufficiently high enough value (based on the thermal conductivities and the model size) to model perfect contact with minimal thermal resistance. Note that the option is not valid for composite materials. For orthotropic materials, the application only considers Thermal Conductivity in the X direction. |
| Manual | The Thermal Conductance Value is input directly by the user. |
Allows input of the Thermal Conductance Value. Only positive values are allowed. This choice is displayed only if Manual is specified for Thermal Conductance. The Units for this value are based on the types of contact involved. For 3D faces and 2D edges, the units are HEAT/(TIME * TEMPERATURE* AREA). For contact between 3D edges and vertices, the units are HEAT/(TIME * TEMPERATURE) with the value applied to every node in the contact side. For more information about the units used for thermal contact conductance coefficient, see Table 78 and Table 79 in the Solving Units section.
For additional Mechanical APDL specific information, see the Modeling Thermal Contact, specifically Modeling Conduction>Using TCC, section of the Mechanical APDL Contact Technology Guide (Multiphysics Contact).
This option enables you to specify the contact search size, commonly referred to as the Pinball Region. Setting a pinball region can be useful in cases where initially, bodies are far enough away from one another that, by default, the program will not detect that they are in contact. You could then increase the pinball region as needed. Consider an example of a surface body that was generated by offsetting a face of a solid body, possibly leaving a large gap, depending on the thickness. Another example is a large deflection problem where a considerable pinball region is required due to possible large amounts of over penetration. In general though, if you want two regions to be bonded together that may be far apart, you should specify a pinball region that is large enough to ensure that contact indeed occurs.
For bonded and no separation contact types, you must be careful in specifying a large pinball region. For these types of contact, any regions found within the pinball region will be considered to be in contact. For other types of contact, this is not as critical because additional calculations are performed to determine if the two bodies are truly in contact. The pinball region defines the searching range where these calculations will occur. Further, a large gap can transmit fictitious moments across the boundary.
Property options include:
|
Property |
Description |
| Program Controlled | This is the default setting. The pinball region will be calculated by the program. |
| Auto Detection Value | This option is only available for contacts generated automatically. The pinball region will be equal to the tolerance value used in generating the contacts. The value is displayed as read-only in the Auto Detection Value field. Auto Detection Value is the recommended option for cases where the automatic contact detection region is larger than a Program Controlled region. In such cases, some contact pairs that were detected automatically may not be considered in contact for a solution. |
| Radius |
The radius value is input directly by the user. |
For the Rigid Body Dynamics solver: In the Rigid Body Dynamics solver, the pinball region is used to control the touching tolerance. By default, the Rigid Body Dynamics solver automatically computes the touching tolerance using the sizes of the surfaces in the contact region. These default values are sufficient in most of cases, but inadequate touching tolerance may arise in cases where contact surfaces are especially large or small (small fillet for instance). In such cases, the value of the touching tolerance can be directly specified using the following properties:
|
Property |
Description |
| Program Controlled (default) |
The touching tolerance is automatically computed by the Rigid Body Dynamics solver from the sizes of the contact surfaces. |
| Radius |
The value of the touching tolerance is directly given by user. |
The numerical value for the Pinball Radius. This choice is displayed only if Pinball Region is set to Radius.
Controls the electric contact conductance value used in an electric contact simulation.
Property options include:
|
Property |
Description |
| Program Controlled |
This is the default setting. The program will calculate the value for the electric contact conductance. The value will be set to a sufficiently high enough value (based on the electric conductivities and the model size) to model perfect contact with minimal electric resistance. |
| Manual |
The Electric Conductance Value is input directly by the user. |
Note: The Electric Analysis result, Joule Heat, when generated by nonzero contact resistance is not supported.
Allows input of the Electric Conductance Value (in units of electric conductance per area). Only positive values are allowed. This choice is displayed only if Manual is specified for Electric Conductance.
Allows you to specify if changes in contact behavior should control automatic time stepping. This choice is displayed only for nonlinear contact (Type is set to Frictionless, Rough, or Frictional).
Property options include:
|
Property |
Description |
|
None |
This is the default setting. Contact behavior does not control automatic time stepping. This option is appropriate for most analyses when automatic time stepping is activated and a small time step size is allowed. |
|
Automatic Bisection |
Contact behavior is reviewed at the end of each substep to determine whether excessive penetration or drastic changes in contact status have occurred. If so, the substep is reevaluated using a time increment that is bisected (reduced by half). |
|
Predict for Impact |
Performs same bisection on the basis of contact as the Automatic Bisection option and also predicts the minimal time increment needed to detect changes in contact behavior. This option is recommended if you anticipate impact in the analysis. |
|
Use Impact Constraints |
Activates impact constraints with automatic adjustment of the time increment. This option includes constraints on penetration and relative velocity to more accurately predict the duration of impact and the rebound velocities after separation. |
For the ANSYS Rigid Dynamics solver, the Advanced group has only one property, Restitution Value. This value represents the energy lost during shock and is defined as the ratio between relative velocity prior to the shock and the velocity following the shock. This value can be between 0 and 1. A Restitution Factor equal to 1 indicates that no energy is lost during the shock, that is, the rebounding velocity equals the impact velocity (a perfectly elastic collision). The default value is .