The following are the tabs on the Contact Properties dialog box for creating a contact pair.
Note: Not all of the above tabs will be available at all times. The tabs that are presented in the GUI and the options shown on each tab will vary depending on the type of contact pair you define, and the location from which you access the Contact Properties dialog (from the Contact Wizard or from the Contact Manager).
Contact Properties: Basic
The Basic tab contains general properties related to contact behavior and convergence.
You should first try running your contact analysis using the default settings, then change settings only if you encounter difficulties or have special situations in your analysis.
Use the questions below to assist you in determining if you need to change any of the default settings based on special situations.
These questions are intended only as hints to guide you in your decision to adjust any of the contact properties and may not cover all possible uses of these parameters. You are advised to review the information in the linked sections (shown below) even if the questions do not apply directly to your situation. The linked sections provide a more complete description on how the parameters can be used.
For this dialog box, the <auto> option indicates that you are choosing a default value, the factor radio button indicates that you are setting a scaling factor, and the constant radio button indicates that you are setting a constant.
| Question | Adjust this tab entry ... |
|---|---|
|
Are you modeling slender structures or other bending dominated problems? | |
|
Does your model exhibit a highly varying mesh density? Does your solution diverge due to chattering? | Penetration tolerance [FTOLN] |
|
Are you experiencing spurious contact because a target segment is far from a contact element, even though penetration exists? | Pinball region [PINB] |
|
Is the contact surface behavior other than standard unilateral contact (that is, other than when normal pressure equals zero if separation occurs)? | Behavior of contact surface [KEYOPT(12)] |
|
Do you need to account for large strain effects (for example, necking down) that change the underlying element's stiffness? Do you need to update the normal or tangential contact stiffness more often than at each load step? | Contact stiffness update [KEYOPT(10)] |
|
Does your model have very distorted elements, a high coefficient of friction, and/or poor convergence behavior when using the default augmented Lagrange method? | Contact algorithm [KEYOPT(2)] |
|
Do you need to build multipoint constraints (MPC) for assemblies? | Contact algorithm [KEYOPT(2) = 2] |
|
Is the amount of penetration in your model not acceptable? | Contact algorithm [KEYOPT(2) = 3, 4] |
|
If you are using the Lagrange/penalty algorithm (KEYOPT(2) = 3) or pure Lagrange multiplier method (KEYOPT(2) = 4), does your solution diverge due to chattering? | Allowable tensile contact pressure [TNOP] |
|
Are you modeling corner, point-to-surface, or edge-to-surface contact and using CONTA172 or CONTA174? | Location of contact detection [KEYOPT(4)] |
|
Is the contact region smoother than the target surface (using CONTA175)? | Contact normal [KEYOPT(4)] |
|
If you are using the MPC algorithm, do you need to constrain any rotational degrees of freedom? | Type of constraint [TARGE170, KEYOPT(5)] |
Related Elements: — CONTA172, CONTA174, CONTA175
Contact Properties: Friction
The Friction tab contains parameters related to static and dynamic friction at the contact interface.
You should first try running your contact analysis using the default settings, then change settings only if you encounter difficulties or have special situations in your analysis.
Use the questions below to assist you in determining if you need to change any of the default settings based on special situations.
These questions are intended only as hints to guide you in your decision to adjust any of the contact properties and may not cover all possible uses of these parameters. You are advised to review the information in the linked sections (shown below) even if the questions do not apply directly to your situation. The linked sections provide a more complete description on how the parameters can be used.
For this dialog box, the <auto> option indicates that you are choosing a default value, the factor radio button indicates that you are setting a scaling factor, and the constant radio button indicates that you are setting a constant.
The Material ID and Friction Coefficient entries replicate the entries on the Contact Properties: Set Parameters and Create dialog box. Use these entries on the Friction tab to create a new material ID or to enter a revised friction coefficient that will overwrite the existing one. (Note that only isotropic friction is available through this dialog box. See Choosing a Friction Model for information on how to define orthotropic friction, which is available for 3D contact only.)
| Question | Adjust this tab entry ... |
|---|---|
|
Does your analysis involve tangential (sliding) contact stiffness that is significantly different from the normal contact stiffness? | Tangent penalty stiffness [FKT] |
|
Are you updating contact stiffness at each iteration [KEYOPT(10) = 0, 2] and have a need to enhance convergence even though accuracy may be compromised? | Allowable elastic slip [SLTO] |
|
Do you need to include sliding resistance in your simulation when there is zero normal pressure? | Contact cohesion [COHE] |
|
Does your analysis involve a bulk metal forming process or similar situation where the contact pressure can become very large? | Maximum friction stress [TAUMAX] |
|
Do frictional stresses have a substantial influence on the overall displacement field? Is the magnitude of the frictional stresses highly solution dependent? Are you having convergence problems with contact simulations that involve friction? | Stiffness matrix [NROPT ] |
|
Are the static and dynamic coefficients of friction unequal? | Static/dynamic ratio [FACT] |
|
If the static and dynamic coefficients of friction are unequal, should a friction decay time be simulated? | Exponential decay coefficient [DC] |
Related Elements: — CONTA172, CONTA174, CONTA175
Contact Properties: Initial Adjustment
The Initial Adjustment tab contains advanced penetration and surface offset parameter settings.
You should first try running your contact analysis using the default settings, then change settings only if you encounter difficulties or have special situations in your analysis.
Use the questions below to assist you in determining if you need to change any of the default settings based on special situations.
These questions are intended only as hints to guide you in your decision to adjust any of the contact properties and may not cover all possible uses of these parameters. You are advised to review the information in the linked sections (shown below) even if the questions do not apply directly to your situation. The linked sections provide a more complete description on how the parameters can be used.
For this dialog box, the <auto> option indicates that you are choosing a default value, the factor radio button indicates that you are setting a scaling factor, and the constant radio button indicates that you are setting a constant.
|
Does your model contain an initial geometric penetration such that contact forces would immediately be "stepped" to a large value (such as an interference fit)? | Initial penetration [KEYOPT(9)] |
|
Are you modeling initial interference contact problems (such as shrink fit assemblies)? | Contact surface offset [CNOF] |
|
Do you need to prevent rigid body motion before contact occurs? | Automatic contact adjustment [KEYOPT(5)] |
|
Do you need to prevent rigid body motion before contact occurs? | Initial contact closure [ICONT] |
Related Elements: — CONTA172, CONTA174, CONTA175
Contact Properties: Miscellaneous
Use the Miscellaneous tab to specify the following settings for your contact analysis.
If the factor button is checked, the value entered into the field is used as a scaling factor. If the constant button is checked, the value entered is used as a constant.
- Contact opening stiffness
This sets a constant value or scaling factor for the FKOP real constant. For modeling either no-separation or bonded contact, you may need to set this value. This provides a stiffness factor applied when contact opens. If a constant value is not selected, the true contact opening stiffness equals FKOP* the contact stiffness applied when contact closes. The default FKOP value is 1.
No separation and bonded contact generate a "pull-back" force when contact opening occurs, and that force may not completely prevent separation. To reduce separation, define a larger value for FKOP. Also, in some cases separation is expected but a connection must be maintained to prevent rigid body motion. In such instances, you can specify a small value for FKOP to maintain the connection between the contact surfaces while allowing separation to occur (this is a "weak spring" effect). This setting is ignored for Standard and Rough settings for Behavior of contact surface (Basic tab).
- Target edge extension factor
This sets the value for real constant TOLS, which is used to add a small tolerance that will internally extend the edge of the target surface. TOLS is expressed in percentage units. A small value is usually efficient. The default value is 10 for small deflection and 2 for large deflection.
- Pressure penetration criterion
When a fluid pressure penetration load is applied at the contact interface, the pressure penetration criterion (real constant PPCN) is used to determine when the pressure penetrates. When the contact pressure is less than the criterion, fluid pressure starts to penetrate. When the contact pressure is greater than the criterion, fluid pressure is cut off.
- Fluid penetration acting time
When a fluid pressure penetration load is applied at the contact interface, the fluid pressure can be ramped linearly over a time period, during one or several substeps. To implement this ramping option, enter a fluid penetration acting time (real constant FPAT). You can enter a fraction of the time increment of the load step (factor) or an absolute acting time (constant).
- Fluid penetration load remains constant
When a fluid pressure penetration load is applied at the contact interface, you can indicate whether the fluid penetration load varies during iterations based on the current contact status (default), or whether it remains constant over the substep.
- Asymmetric contact selection
When there are several contact pairs involved in the model, and the graphical picking of contact and target surfaces is difficult, you can just define the symmetric contact pairs. When you choose this option, the program internally selects which asymmetric pairs are to be used at the solution stage.
- Beam/shell thickness effect
By default, Mechanical APDL does not account for the element thickness, beams and shells are discretized at their mid-surface, and the penetration distance is calculated from the mid-surface. You can account for the thickness of shells (2D and 3D) and beams (2D) by using this option. When this option is active, the distance of contact is calculated from either the top or the bottom surface and
For rigid-to-flexible contact, the program will automatically shift the contact surface to the bottom or top of the shell/beam surface.
For flexible-to-flexible contact, the program will automatically shift both the contact and target surface (if they are attached to shell/beam elements).
When building your model geometry, if you are going to account for thickness, remember the offsets which may come from either contact surface or target surface or from both. When you specify a contact offset and activate this option, it is defined from the top or bottom of the shell/beam, not the mid-surface. When used with SHELL181, SHELL208, or SHELL209, changes in thickness during deformation are also taken into account.
- Element time increment
Time step control is an automatic time stepping feature that predicts when the status of a contact element will change or cuts the current time step back. Select one of four actions to control time stepping:
: The time step size is unaffected by the prediction. This setting is appropriate for most analyses when automatic time stepping is activated and a small time step size is allowed.
: Time step size is bisected if too much penetration occurs during an iteration, or if the contact status changes dramatically.
: Predict a reasonable increment for the next substep.
: Predict a minimal time increment for the next substep.
: Activate energy and momentum conserving contact in transient dynamic analysis.
- Superelement usage
The surface-to-surface contact elements can model a rigid body (or one linear elastic body) contacting another linear elastic body undergoing small motions. These elastic bodies can be modeled using superelements, which greatly reduces the number of degrees of freedom involved in the contact iteration. Remember that any contact or target nodes must be one of the master nodes of the superelements.
Since the superelement consists only of a group of retained nodal degrees of freedom, it has no surface geometry on which Mechanical APDL can define a contact and target surface. Therefore, the contact and target surface must be defined on the surface of the original elements before they are assembled into a superelement. Information taken from the superelement includes nodal connection and assembly stiffness, but no material property or stress states (whether axisymmetric, plane stress, or plane strain). One restriction is that the material property set used for the contact elements must be the same as the one used for the original elements before they were assembled into superelements.
The following selections are valid:
- The thickness (real constant R2) is set through the field below.
Note: The above bulleted options are not available if you are using CONTA175. However, the Contact Wizard does provide the Contact Model capability, which allows you to base the contact model either on contact force or contact traction.
Contact model -- For the CONTA175 element, the contact model can be either contact force based (KEYOPT(3) = 0, default) or contact traction based (KEYOPT(3) = 1). For the contact traction based model, Mechanical APDL can determine the area associated with contact nodes. For the single point contact case, a unit area will be used which is equivalent to the contact force based model.
Contact Properties: Rigid Target
Use the Rigid target tab to specify the following settings for your contact analysis.
- Boundary condition on target nodes
The boundary conditions on the target can be either automatically constrained or user specified.
For the Auto constrained option (the default), the program checks the boundary conditions for each target surface. If all of the conditions listed below are met, then Mechanical APDL treats the target nodes along the respective degree of freedom as fixed:
There are no explicit boundary conditions or prescribed forces for target surface nodes.
Target surface nodes are not connected to other elements.
No constraint equations or node couplings have been used to constrain target surface nodes.
At the end of each load step, the program releases the constraint conditions that were set internally.
The constraint conditions stored in the result file (Jobname.rst) and the database file (Jobname.db) may be updated due to this change. You should carefully verify whether the current constraint conditions are as expected before restarting an analysis or resolving the problem in interactive mode.
If you wish to control the constraint conditions of target nodes, select User specified.
- Area elements have
Defines whether 3–D rigid target surfaces were meshed with high-order (midside nodes) or low-order target elements.
- Pilot Node
You can define or modify the pilot node using these options:
Pilot Name (optional) - You can specify a name for a nodal component that will contain the pilot node. This allows easier interaction with the pilot node later on.
Pilot Node - You can create or modify (delete/move) a pilot node using one of the listed methods. The definition methods include an automatic method (at centroid of target elements), picking methods (pick existing keypoint, node, or working plane location), and direct input of coordinates in the active coordinate system. Pick to launch the pilot node location picker or input the node coordinates. The pilot node is not created or modified until after you pick in the Contact Properties dialog.
Contact Properties: Thermal
Use the Thermal tab to specify the following settings for your contact analysis.
- Thermal Contact Conductance
This sets the real constant TCC.
The conductive heat transfer between two contacting surfaces is given by:
q = TCC X (Tt - Tc)
where:
q is the heat flux per area, TCC is the thermal contact conductance coefficient, and Tt and Tc are the temperatures of the contact points on the target and contact surfaces. TCC can be input as a constant value or as a table. In a table, TCC can be a function of temperature, pressure, time, and location. The drop-down list box lists all tables that have been defined.
- Stephan-Boltzmann constant
This sets the real constant SBCT used to model radiation.
Heat transfer through radiation is given by:
q = RDVF x EMIS x SBCT [(Te + TOFFST)4 - (Tc + TOFFST)4]
where: TOFFST is the temperature offset from absolute zero to zero (defined through the TOFFST command.) EMIS is the surface emissivity. RDVF is the radiation view factor. - Radiation View factor
This sets the real constant RDVF. The radiation view factor can be input as a constant value or as a table. In a table, RDVF can be a function of temperature, gap distance, time, and location. The drop-down list box lists all tables that have been defined.
- Emissivity
This sets the surface emissivity (MP,EMIS).
- Frictional heating factor
This sets the real constant FHTG used to model heat generation due to frictional sliding.
The rate of frictional dissipation is given by:
q = FHTG x τ x V
where: τ is the equivalent frictional stress. V is the sliding rate. FHTG is the fraction of frictional dissipated energy converted into heat (defaults to 1). - Dissipation weight factor
This sets the real constant FWGT used to model heat generation due to frictional sliding. It is the weight factor for the distribution of heat between the contact and target surfaces (defaults to 0.5).
The amount of frictional dissipation on contact and target surfaces is given by:
qc = FWGT x FHTG x τ x V
and
qT = (1 - FWGT) x FHTG x t x V
where: qc is the amount of frictional dissipation on the contact side. qT is the amount of frictional dissipation on the target side FWGT defaults to 0.5. - Thermal contact behavior
This sets KEYOPT(3) for target elements TARGE169 and TARGE170. There are two options for thermal contact behavior:
Based on Contact Status (KEYOPT(3) = 0). This is the default option.
Treated as Free Surface (KEYOPT(3) = 1).
For KEYOPT(3) = 0, the thermal contact behavior depends on contact status as follows:
Closed Contact -- Thermal contact conduction transfers heat between two contacting surfaces.
Frictional Sliding -- Frictional dissipated energy generates the heat to both the contact and target surfaces.
Near-Field Contact -- Both heat convection and radiation between the contact and target surfaces is taken into account. The external flux value contributes to the contact surface.
Far-Field Contact -- Heat convection and radiation between the contact surface and the environment is taken into account. The external flux value only contributes to both contact and target surfaces.
If you choose the free surface contact behavior, Mechanical APDL considers both free surface radiation and convection as long as open contact is detected. In this case, there is no convection or radiation heat transfer between the contact and target surfaces.
Contact Properties (Constraint Type): Constraint
The Constraint tab contains general parameters related to the behavior of surface-based constraint contact pairs. Surface-based constraints are used to couple the motion of nodes on the contact surface to a single pilot node on the target surface. A surface-based constraint requires the multipoint constraint (MPC) contact algorithm (KEYOPT(2) = 2). (This KEYOPT is set automatically if you use the Contact Wizard to create the contact pair.)
- Constraint surface type
When the multipoint constraint (MPC) algorithm is used, KEYOPT(4) determines the surface-based constraint type. Two types are available:
Force-distributed constraint surface - In this type of constraint, forces or displacements applied on the pilot node are distributed to contact nodes (in an average sense) through shape functions (similar to a constraint defined by the RBE3 command).
Rigid constraint surface - In this type of constraint, the contact nodes are constrained to the rigid body motion defined by the pilot node (similar to a constraint defined by the CERIG command).
- Boundary conditions on target
The boundary conditions on the target node can be either automatically constrained or user specified.
For the Auto constrained option (the default), the program checks the boundary conditions for the target node. If all of the conditions listed below are met, then Mechanical APDL treats the target node along the respective degree of freedom as fixed.
There are no explicit boundary conditions or prescribed forces for the target node.
The target node is not connected to other elements.
No user-specified constraint equations or node couplings have been used to constrain the target node.
At the end of each load step, Mechanical APDL releases the constraint conditions that were set internally.
The constraint conditions stored in the result file (Jobname.rst) and the database file (Jobname.db) may be updated due to this change. You should carefully verify whether the current constraint conditions are as expected before restarting an analysis or resolving the problem in interactive mode.
If you wish to control the constraint conditions of the target node, select User specified.
- Constrained DOF set on target
KEYOPT(4) of the target element is used to specify the degrees of freedom to be constrained. A checked box indicates the DOF is active, and an empty box indicates the DOF is inactive.
- Pilot Node
You can modify the pilot node using these options:
Pilot Name (optional) - You can specify a name for a nodal component that will contain the pilot node. This allows easier interaction with the pilot node later on.
Pilot Node - You can modify a pilot node using one of the listed methods. The definition methods include an automatic method (at centroid of contact elements), picking methods (pick existing keypoint, node, or working plane location), and direct input of coordinates in the active coordinate system. Pick to launch the pilot node location picker or input the node coordinates. The pilot node is not modified until after you pick in the Contact Properties dialog.
Contact Properties: ID
Use the Identification tab to specify ID numbers for your contact pair. By default Mechanical APDL will assign the numbers shown in the various fields.
- Contact pair real set ID
A contact pair must share the same real constant set number. You can use this field to assign any number that you wish, or accept the value shown. After the contact pair is created, you cannot change this number.
- Target element type ID
Mechanical APDL automatically creates this ID.
- Contact element type ID
Mechanical APDL automatically creates this ID.
If you are creating symmetric contact pairs in the Contact Wizard, the following fields are also shown.
- Companion contact pair real set ID
The companion pair must use a different real constant set number. You can use this field to assign any number that you wish, or accept the value shown. After the contact pair is created, you cannot change this number.
- Companion target element type ID
Mechanical APDL automatically creates this ID.
- Companion contact element type ID
Mechanical APDL automatically creates this ID.