9.6.3.3. Advanced Settings

The Advanced category provides the following properties.

Formulation

The Formulation property specifies which algorithm the application uses for contact pair computations. Property options include:

Option	Description	Mechanical APDL Reference
Program Controlled (default)	For this setting, the application internally selects the: Pure Penalty option for contact between two rigid bodies. MPC option when the Inverse Option property is set to Yes (Analysis Settings > Advanced). MPC option for bonded contact defined between solid-solid, solid-shell, shell-shell, and shell-beam bodies in 3D structural analyses. Exclusions The application uses the Augmented Lagrange option internally when the analysis: Is a Static Structural that includes Additive Manufacturing processes or DED Process Add On (Extension). If the Physics Type property is set to an option other than Structural, such as Thermal or Acoustics. This property is generally populated based on the analysis type you select, but could vary for a Coupled Field analysis, as shown in the Physics Definition category of the environment. Includes a Cyclic Symmetry object. Is a Substructure Generation analysis. Is linked to a downstream Structural Optimization analysis. Has a contact region scoped to a body that is also scoped to a General Axisymmetric object. If the bonded contact has an edge or a face overlapping with certain boundary conditions, such as Fixed Support, Frictionless Support, Simply Supported, Cylindrical Support, or Displacement as support (at least one entry as zero and other entries set to Free or all entries as zero), and loads such as Remote Force and Remote Displacement. Important: The scoping for the contact regions and boundary conditions in this scenario must be geometry-based. Augmented Lagrange option for all other contact situations.	–
Pure Penalty	Basic contact formulation based on penalty methods.	KEYOPT(2) = 1
Augmented Lagrange	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
MPC	Available for Bonded and for No Separation contact Types. Multipoint Constraint equations are created internally during the Mechanical APDL solution 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
Normal Lagrange	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
Beam	Available for Bonded 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.

Fluid Structure Interface Contact Conditions

Note the following for contact conditions defined at a Fluid Structure Interface:

The Contact side must be on the acoustic body and the Target must be on the structural body.
The Bonded contact type setting and the Pure Penalty formulation is supported in addition to MPC formulation.
Pure Penalty formulation is not supported for contact conditions between two acoustic bodies.
The Nodal-Dual Shape Function Projection (keyo,cid,4,4) option, of the Detection Method property, is used by default for FSI contact defined using the Pure Penalty formulation.
The Combined option (keyo,cid,4,5), of the Detection Method property, is not supported for the MPC formulation type

Small Sliding

The Small Sliding property displays and activates an assumption of relatively-small sliding (less than 20% of the sum of the average length of each contact element for the contact pair). If small sliding is known to occur, this feature can make your solution more efficient and robust. The Program Controlled setting for the Small Sliding property automatically sets the property to On in most situations if the Large Deflection property is set to Off or the Type property is set to Bonded contact. The default setting for this property can be changed using the Small Sliding option in the Connections category of the Options preference.

Note: When you specify a Coupled Field analysis using Electrostatic physics only (standalone), the application automatically disables this property.

Property options include:

Option	Description
Program Controlled	This is the default setting. The application determines whether to select small or finite sliding.
Yes	Enable small sliding.
No	Disable small sliding and set finite sliding.
Adaptive	Activates adaptive small sliding.

For additional information, see the Selecting a Sliding Behavior topic in the Mechanical APDL Contact Technology Guide.

Detection Method

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:

Option	Description
Program Controlled	The application uses Gauss integration points (On Gauss Point) when the Formulation property is set to Pure Penalty or Augmented Lagrange. It uses nodal point (Nodal-Normal to Target) when the Formulation property is set to MPC or Normal Lagrange. When the contact side is scoped to Gasket bodies, the application automatically selects the option, Nodal-Projected Normal From Contact.
On Gauss Point	The contact detection location is at the Gauss integration points. This option is not applicable to contacts with MPC or Normal Lagrange formulation.
Nodal - Normal From Contact	The contact detection location is on a nodal point where the contact normal is perpendicular to the contact surface.
Nodal - Normal To Target	The contact detection location is on a nodal point where the contact normal is perpendicular to the target surface.
Nodal - Projected Normal From Contact	The contact detection location is at contact nodal points in an overlapping region of the contact and target surfaces (projection-based method). Note: Additive Manufacturing Process simulations do not support projection-based contact.
Nodal - Dual Shape Function Projection	The contact detection location is at contact nodal points in an overlapping region of the Contact and Target surfaces (Dual Shape function projection-based method). This option is efficient in terms of solution performance and memory usage and generally remedies potential over constraint due to MPC equations.
Combined	The Mechanical APDL solver will use the optimized detection approach based on the bodies in contact.

For additional Mechanical APDL information, see Selecting Location of Contact Detection (specifically, KEYOPT(4) related information) in the Mechanical APDL Contact Technology Guide.

Penetration Tolerance

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 Program Controlled, Pure Penalty, or Augmented Lagrange.

Note: The Update Stiffness property must be set to either Program Controlled, Each Iteration, or Each Iteration, Aggressive for the Penetration Tolerance property to be displayed when Formulation is set to Pure Penalty.

Property options include:

Option	Description
Program Controlled (default)	The Penetration Tolerance is calculated by the application.
Value	Enter the Penetration Tolerance Value directly. This entry is a length measurement (foot, meter, etc.). Only non-zero positive values are valid.
Factor	Enter the Penetration 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.

Penetration Tolerance Value

The Penetration Tolerance Value property displays when Penetration Tolerance is set to Value. You enter a Value.

Penetration Tolerance Factor

The Penetration Tolerance Factor property displays when Penetration Tolerance is set to Factor. You enter a Factor.

Note: When viewing the Connections Worksheet, a Value displays as a negative number and a Factor 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).

Elastic Slip Tolerance

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 Each Iteration or Each Iteration, Aggressive).

Note: Elastic Slip Tolerance is not applicable when the contact Type is set to Frictionless or No Separation.

Property options include:

Option	Description
Program Controlled (default)	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 Value. You enter a Value.

Elastic Slip Tolerance Factor

The Elastic Slip Tolerance Factor property displays when Elastic Slip Tolerance is set to Factor. You enter a Factor.

Note: When viewing the Connections Worksheet, a Value displays as a negative number and a Factor 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).

Constraint Type

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. The property includes the following options:

Option	Description
Program Controlled (default)	Internally, this setting corresponds to the: Projected, Displacement Only option for General Axisymmetric contact and for contact between rigid and deformable bodies. Distributed, All Directions option for all edge-to-edge contacts and for contacts which are not scoped to solid bodies on both contact side and target side. For all other contact conditions, automatic constraint type detection is performed internally by the solver. See the description for KEYOPT(5) in the TARGE170 element section of the Mechanical APDL Element Reference for a listing of the internal settings. Recommendation: When you have multiple bonded contacts using the MPC formulation with a common contact or target scoping, Ansys recommends that you merge such contacts into single contact, to avoid possible over constraint issues.
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. Therefore, 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. Therefore, 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.

Normal Stiffness

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 of the program controlled regions (including Bonded or No Separation) will use the Mechanical APDL default (Real Constant FKN).
Factor	You enter the Normal Stiffness Factor (see below). This is a unit-less entry.
Absolute Value	You enter the Normal Stiffness Value (see below).

Normal Stiffness Factor

This property appears when the Normal Stiffness property is set to Factor. It enables you to specify the Normal Stiffness Factor. Only non-zero positive values are supported. The usual factor range is from 0.01 - 10The default value is selected by the application. 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 information specific to Mechanical APDL, see the following sections:

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).

Normal Stiffness Value

This property appears when the Normal Stiffness property is set to Absolute Value. It enables you to specify the Normal Stiffness Value. The application supports positive values only. The Units for this value are based on the types of contact involved. For a traction based model, the application uses Force/Volume (for example, N/m³) and for a force-based model, the application uses Force/Length (for example, N/m). A force-based model is used for face-to-edge contacts and edge-to-edge (not including line bodies).

Update Stiffness

This property 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 application modifies the stiffness (raise/lower/leave unchanged) based on the physics of the model (that is, the underlying element stress and penetration). To use the options of this property, you need to set the Formulation property to either Augmented Lagrange or Pure Penalty, the two formulations where contact stiffness is applicable. For the Each Iteration, Exponential option, the Formulation property must be set to Pure Penalty.

An advantage of specifying an Update Stiffness setting 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:

Option	Description
Program Controlled	This is the default setting. The application sets the property to Never for contacts between two rigid bodies and to Each Iteration for all other cases. You can change the default using the Options dialog.
Never	This is the default setting. Turns off the program's automatic Update Stiffness feature.
Each Iteration	Sets the program to update stiffness at the end of each equilibrium iteration. This choice is recommended if you are unsure of a Normal Stiffness Factor to use in order to obtain good results.
Each Iteration, Aggressive	Sets the program to update stiffness at the end of each equilibrium iteration, but compared to the Each Iteration, this option allows for a more aggressive changing of the value range.
Each Iteration, Exponential	This option requires the Type property to be set to either Frictional or Frictionless and the Formulation property to Pure Penalty. When selected, the Pressure at Zero Penetration and the Initial Clearance properties display. This option updates stiffness using an exponential pressure-penetration relationship. For detailed information about this option, see the Exponential Pressure-Penetration Relationship (KEYOPT(6) = 3) topic (of the Set the Real Constants and Element KEYOPTS section) in the Mechanical APDL Contact Technology Guide.

Electric Capacitance

This property controls the electric contact capacitance value used in an electric contact simulation. Property options are described below.

Option	Description
Program Controlled	This is the default setting. Using this setting, the application calculates the value for the electric contact capacitance. The value is calculated based on the maximum value of the average of permittivity and the size of the model. For orthotropic materials, the application only considers Relative Permittivity in the X direction.
Manual	You use this setting to specify an electric capacitance value.

Electric Capacitance Value

This property displays when you set the Electric Capacitance property to Manual. You use this property to specify a Electric Capacitance Value (positive values only).

Pressure at Zero Penetration

This property corresponds to the PZER real constant used in the Mechanical APDL application. It defines the pressure when there is zero penetration between Contact and Target geometries. See the Exponential Pressure-Penetration Relationship (KEYOPT(6) = 3) topic (of the Set the Real Constants and Element KEYOPTS section) in the Mechanical APDL Contact Technology Guide for a detailed description of this property and its function. Property options are illustrated and described below.

Option	Description	Mechanical APDL Reference
Program Controlled	This is the default setting. The application automatically calculates and selects default pressure values.	KEYOPT(6) = 3
Value	Using this option, you can manually specify a pressure value. This entry has a unit of measure for pressure (Pa, etc.). Only non-zero positive values are valid.
Factor	Using this option, you can manually specify a factor of the default pressure value. This entry must be equal to or greater than zero but must also be less than 1.0. This entry has no unit.

Initial Clearance

This property corresponds to the CZER real constant used in the Mechanical APDL application. It defines the initial clearance or gap at which the contact pressure begins to act on the Contact and Target geometries. See the Exponential Pressure-Penetration Relationship (KEYOPT(6) = 3) topic (of the Set the Real Constants and Element KEYOPTS section) in the Mechanical APDL Contact Technology Guide for a detailed description of this property and its function. Property options are illustrated and described below.

Option	Description	Mechanical APDL Reference
Program Controlled	This is the default setting. The application automatically calculates and selects default clearance values.	KEYOPT(6) = 3
Value	Using this option, you can manually specify a clearance value. This entry is a length measurement (meter, etc.). Only non-zero positive values are valid.
Factor	Using this option, you can manually specify a factor of the default clearance value. This entry must be equal to or greater than zero but must also be less than 1.0. This entry has no unit.

Stabilization Damping Factor

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 the Frictionless, Rough, and Frictional options of the Type property. 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 are described below.

Option	Description	Mechanical APDL Reference
Stabilization Damping Factor	If the value provided for the damping factor is: `0` (default value), damping is activated for the first load step only. The solver uses a default value of `1.0` as the Stabilization Damping Factor. Non-zero, then damping is always activated regardless of the contact status of the previous substeps. The solver uses (KEYOPT(15) = 3) to apply stabilization damping.	Real Constant FDMN

Thermal Conductance

Controls the thermal contact conductance value used in a thermal contact simulation. Property options are described below.

Option	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 Program Controlled 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.

Option

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 Program Controlled 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.

Thermal Conductance Value

This property displays when the Thermal Conductance property is set to Manual. Enables entry of the Thermal Conductance Value. The property only supports positive values and can be specified as a parameter. 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).

Pinball Region

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 application does not detect that they are in contact. In this case, you can increase the pinball region. For example, you could have a surface body that was generated by offsetting a face of a solid body. Depending upon the thickness, this could leave a large gap. Or, for a large deflection problem, a considerable pinball region to compensate for the possibility of large amounts of over penetration. In general, 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 occurs.

However, for the Bonded and No Separation contact types, you must be careful when specifying a large Pinball Region. For these types of contact, the application considers any region found within the pinball region to be in contact. For the other contact types, this consideration is not as critical because the application performs additional calculations to determine if the two bodies are truly in contact. The pinball region defines the searching range where these calculations will occur. In addition, a large gap can transmit fictitious moments across the boundary.

Property options include:

Option	Description
Program Controlled	This is the default setting. The application calculates the Pinball Region value.
Auto Detection Value	This option is only available for automatically generated contacts. 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	When selected, the Pinball Radius property displays. You use this property to manually specify a radius value.

Rigid Dynamics Solver

For the Rigid Dynamics solver, the Pinball Region property is used to control the touching tolerance. By default, the Rigid 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:

Option	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.

Pinball Radius

The numerical value for the Pinball Radius. This property is displayed only if Pinball Region is set to Radius.

Electric Conductance

Controls the electric contact conductance value used in an electric contact simulation. Property options are described below.

Option	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.

Electric Conductance Value

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.

Time Step Controls

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 are described below.

Option	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.

Restitution Factor—Rigid Dynamics Solver Only

For the Ansys Rigid Dynamics solver, Restitution Value is a property in the Advanced group. This value represents the energy lost during shock. It is defined as the ratio between relative velocity prior to the shock and the velocity after 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 1.

Continuous Distance Computation—Rigid Dynamics Solver Only

For the Ansys Rigid Dynamics solver, Continuous Distance Computation is an additional property in the Advanced group. This property continuously computes the contact distance during the simulation. By default, the distance is only computed when the contact bodies are significantly close in contact. However, it can force distance computation, even when contact bodies are distant. Enabling Continuous Distance Computation is mandatory in order to monitor the distance between contact bodies (see Contact Distance Probes for further information). The Continuous Distance Computation property can be defined as Program Controlled. Select either Yes to enable distance computation or No to disable it. The default value is Program Controlled, which disables the distance computation.