Contact Parameters dialog box (Simcenter Samcef)

Use this dialog box to create a Contact Parameters modeling object.

Modeling Object
Name	Sets a unique name for the modeling object.
Label	Sets a unique integer for the modeling object.This label also appears in the Modeling Objects Manager dialog box, and you can filter the objects listed in that dialog box by their label.
Properties
Solution Applicability View	Specifies the solution type whose parameters you want to display on the dialog box. Only the Nonlinear Analysis and Linear Static Analysis Samcef solution types have corresponding contact parameters.
Iteration Method	Appears when Solution Applicability View is set to All Solutions or Nonlinear Analysis.Specifies the iteration method for making the contact.CoupledAvailable only in a Nonlinear Analysis. Processes the contact degrees of freedom with all of the other degrees of freedom in the model.UncoupledProcesses the contact degrees of freedom separately from all of the other degrees of freedom in the model.Note: We do not recommend any uncoupled methods in nonlinear analyses if you define a Bidirectional contact.For more information, see the OPT parameter of the Samcef .MCT command.

General Parameters page

Surface Selection Options
Displacement Formulation (NLIM)	Specifies the displacement formulation (sliding), which determines whether contact conditions are updated. DefaultThe solver chooses the most appropriate formulation. For a Nonlinear Analysis, the default is Large Displacement. For a Linear Static Analysis, default is Small Displacement.Large DisplacementsContact conditions are updated. When large displacement (sliding) occurs, the contact node slides from one element face to the element face of another element. Tracking the moves from one element to another requires additional computation time.Small DisplacementsContact conditions are not updated. This option assumes that the contact node remains in contact with the initial element face. Therefore, contact conditions do not require updating, which saves computation time.For more information, see the NLIM parameter of the Samcef .MCT command.
Topology Search (UN2)	Specifies how to compute the number of Target Region element faces that must be taken into account in the contact equation. By default, for each Source Region node, the software automatically computes the number of Target Region element faces that must be taken into account in the contact equation.**Compute At Each Iteration (UN2 3)**Perform this computation at each iteration of the contact process. This option is more CPU intensive and is recommended in most of the contact conditions, especially for large displacements.**Compute At Each Time Step (UN2 2)**Perform this computation once for each time step.DefaultPerform this computation only at the pre-processing stage. This option is less CPU intensive but is only suitable for small displacements.For more information, see the UN2 parameters of the Samcef .MCT command.
Extension Factor (EXT)	Sets the factor for extending the contact surfaces beyond their boundaries. The length of this extension is the length of the contact segment multiplied by this value. This is an advanced option for enlarging the faces close to an edge so that more nodes are in contact with it, and for ensuring that a node remains in contact with an element even if it moves slightly.
Contact Surfaces (SHEL)	Specifies whether the contact surfaces are single-sided or double-sided for 3D contact. This option has no effect for 2D contact.Select Double-Sided for shell elements for which you want the contact to be taken into account from both sides of the shell. In this case, regardless of the side of the node, the contact is prohibited from going to the other side of the shell.
Contact Characteristics
Contact Regions Tying in Normal Direction (OPCO)	Appears when Solution Applicability View is set to Nonlinear Analysis and Iteration Method is set to Coupled.Specifies whether the contact regions in each contact pair are tied together in a normal direction. Tied means that the contact works both in traction and in compression (like gluing in the normal direction). The classical contact condition only works in compression.Not TiedThe contact can be released. Use for a contact condition that works only in compression. Most contact is not tied. Remains Tied After Contact is ActiveOnce the contact is closed, it remains closed. Use for a contact condition in which the surfaces are not in contact at the start of the computation (for example, due to gaps), but when they do come in contact, you want them to remain in contact and not be separated.TiedThis is a bilateral contact. Use for a contact condition that you want to model as gluing in the normal direction. This option is related to the normal direction and does not affect the tangential direction. The tangential direction is constrained by friction.No Contact, only Contact Separation DistanceUse for a contact condition that you want to model with constant separation in the normal direction.For more information, see the OPCO parameter of the Samcef .MCT command.
Contact Node Tying Tolerance (DLIM)	Appears when Contact Regions Tying in Normal Direction (OPCO) is set to Tied.Sets the minimum distance between the two contact regions.
Continuous Segment Normal (KSMO)	Specifies whether a continuous (that is, interpolated from one element to its neighboring ones) contact segment normal (and associated smoothed surface) is used for the contact surfaces. This option activates smoothing for shell elements or faces of solid elements during contact. Smoothing modifies the topology of elements, like transforming a set of linear elements into parabolic elements with smooth normals between them.Not UsedThe smoothing algorithm is not used. The contact occurs with element normal directions and element topology with no modifications. Used for Single-Sided ContactThe smoothing algorithm is used only for single-sided contact.UsedThe smoothing algorithm is used for both single-sided and double-sided contact. For more information, see the KSMO parameter of the Samcef .MCT command.
Reverse Shell Normal (REVE)	Specifies whether to reverse shell normals during contact computation.Note: When target elements are shells or membranes, the contact algorithm cannot determine where the material is. By default, it assumes that the normal of shells points towards the source nodes. Set Reverse Shell Normal (REVE) to No to change this default.
Topology Search
Maximum Variation of Contact Distance (DGAP)	Appears when Solution Applicability View is set to Nonlinear Analysis and Iteration Method is set to Coupled.In dynamic nonlinear analysis, the automatic time step algorithm can modify the time step to fit the contact requirements.You can use the Maximum variation of Normal Distance (DGAP) option to define the maximum variation of the normal distance between the node and the facet during the time step where the contact occurs. If this criterion is not satisfied, the time step is rejected.For more information, see the DGAP parameter of the Samcef .MCT command.
Contact Characteristic Length (DCON)	Lets you specify the inactive distance above which no contact occurs.For more information, see the DCON parameter of the Samcef .MCT command.

Initial Penetration page

Option	Description
Initial Penetrations/Gaps	Specifies how to handle the initial gap or penetration of the contact elements. By default, if an initial penetration (overlap) or gap exists between the contact source and target, the software attempts to eliminate the penetration or gap. GeometricThe contact starts when the distance between the source node and the target element face is equal to zero.Contact is evaluated exactly as the geometry is modeled. No corrections occur for gaps or penetrations. The list of penetrating nodes is printed, and the minimum and maximum penetrations are written at the beginning of the solve. **Set Penetration to Zero (UN3 1)**The contact starts as soon as the source node moves toward the target element face.Initial penetrations or gaps are ignored. For each node in contact, the initial distance to the target face is considered as the distance at which contact occurs, even if gaps or penetrations exist. Set Gaps and Penetrations to an Interference of DMINInitial penetrations or gaps are overridden by the value for Contact Gap Distance (DMIN). **Set Penetration to Zero for the Closest Node (UN3 2)**Penetrations are reset to a new initial condition in which no interference exists for the closest node.Initial penetrations or gaps are ignored. For each node in contact, the initial distance to the target face is considered as the distance at which contact occurs, even if gaps or penetrations exist. Set Gap or Penetration for the Closest Node to an Interference of DMINGaps and penetrations are both reset to a new initial condition in which DMIN provides an interference for the closest node.See the Samcef .MCT command for more details.
Default Offset Distance for Contact Regions (DMIN)	Appears when Initial Penetrations/Gaps is set to Geometric, Set Penetration to Zero (UN3 1), or Set Penetration to Zero for the Closest Node (UN3 2).Sets the default offset distance for contact regions. Use this option to account for shell thickness. For example, if two shells are in contact, the offset corresponds to the sum of the half thickness of each shell.For more information, see the DMIN parameter of the Samcef .MCT command.
Constant Gap Distance (DMIN)	Appears when Initial Penetrations/Gaps is set to Set Gaps and Penetrations to an Interference of DMIN or Set Gap or Penetration for the Closest Node to an Interference of DMIN.Sets a constant gap distance between the source region (contactor) and the target region when Initial Penetrations/Gaps (INIPENE) is set to Overridden by GAPVAL. A negative number indicates that whatever the distance is between nodes and faces, the contact is assumed to be penetrated by the value you enter, and these penetrations are eliminated.For more information, see the DMIN parameter of the Samcef .MCT command.
Penetration Depth (DCON)	Sets the distance of the penetration or gap to limit contact detection for the target contact surface. The distance must be greater than zero.A contact element is created if the distance is less than or equal to the value you enter.For more information, see the DCON parameter in Topology search in the Samcef .MCT command.
Shell Thickness and Z-Offset (SHTH)	Specifies whether thicknesses and Z-offsets of shells are included in the calculations of the initial penetration of contacting surfaces of shells.Do not IncludeThe software does not include the offset in the calculation. Use this option if: Contact involves only solid elements.Contact involves shell elements, but you already considered the thickness and Z-offset in the Contact Gap Distance (DMIN), specified manually.Include Average OffsetThe software automatically includes the average offset between the shell elements and the outer surfaces of the shells in the calculation. Include Maximum OffsetThe software automatically includes the maximum offset between the shell elements and the outer surfaces of the shells in the calculation. Automatically including the offset is useful when:Contact involves shell elements and no Contact Gap Distance (DMIN) is specified, or the value specified does not consider the shell thickness and Z-offset (if any).A group of shells contains elements with different thicknesses.Computation of Contact Gap Distance (DMIN) for each contact is complicated.For more information, see the SHTH parameter of the Samcef .MCT command.

Normal Behavior page

Regularization Type	Specifies how you want the software to regularize the model. This regularization is for the normal direction. The regularization types define the status of the contact (in contact or open) based on normal distance and a regularization stiffness. By default, the stiffness comes from the mean value of the stiffnesses in the model. But for certain applications that include soft components, you may want to use a value computed per contact (smallest in the contact pairs), or you may want to define it manually.Normal regularization is very helpful, and is likely required for the solution to converge, when the stiffness of the components that are in contact are very different, such as steel in contact with rubber.DefaultUses the default value computed by the solver, which is the stiffness from the mean value of the stiffnesses in the model.No RegularizationSets Normal Regularization Value (PRCS) to -1. No regularization is performed.Computed from Contact SupportsSets Normal Regularization Value (PRCS) to -2, which lets the software use a value computed by the solver. When you select this option, the solver computes a value dedicated to the two supports used for the contact condition. If all of the materials are the same, or if the order of magnitude of the stiffness is the same, selecting this option has no visible effect on how the contact is solved.Automatic ChoiceSets Normal Regularization Value (PRCS) to -3, which lets the software choose the best regularization value.User DefinedLets you define the regularization value. The software uses the value you specify for Normal Regularization Value (PRCS). For more information, see Contact strategies, algorithms, and options (Simcenter Samcef) and the PRCS parameter of the .MCT command.
Normal Regularization Value (PRCS)	Appears when Regularization Type is set to No Regularization, Computed from Contact Supports, Automatic Choice, or User Defined.Displays the normal regularization value that corresponds to the specified Regularization Type. The value is locked and cannot be changed unless you set Regularization Type to User Defined.When Normal Regularization Type is set to User Defined, sets the regularization factor p for the augmented Lagrange multipliers for this specific contact condition.For more information, see the PRCS parameter of the .MCT command.
Normal Stiffness Model Type	Appears when Solution Applicability View is set to Nonlinear Analysis and Iteration Method is set to Coupled.Specifies the method for defining the contact stiffness.DefaultUses hard contact, which is infinite stiffness. Select this option for fully rigid contact.Constant StiffnessUses a basic method that allows you to adjust the contact stiffness by a single value.Constant ComplianceUses a basic method that allows you to adjust the contact stiffness by a single value, but setting an inverse of the stiffness. Nonlinear StiffnessLets you enter a nonlinear function and scale that limits the depth of penetration when pressure increases. For example, to help convergence, you can add stiffness in a contact condition. A constant value ensures that the penetration is proportional to the contact pressure and the stiffness. In some cases, however, you may want to allow penetration for convergence purposes but only to a specified depth. To accomplish this, instead of a constant value, you define the relation between the contact pressure and the normal distance with a table. You can then define a nonlinear function that limits the evolution of the penetration when the pressure increases.Automatic ChoiceUses a value that is computed from the stiffness of both contact supports and the average size of the contact target support.Stiffness from MaterialLets you select the material of the contact parts so that the type of material can be accounted for in computing the stiffness between the two bodies in contact. This option does not apply to Surface-to-Surface contact.For more information, see the THICK parameter of the Samcef .MCT command.
Contact Stiffness (STIF)	Appears when Normal Stiffness Model Type is set to Constant Stiffness.Sets the normal contact modulus to explicitly define the stiffness by a single value adjustment. To define the stiffness, enter a value greater than 1.0E-16.For more information, see the STIF parameter of the Samcef .MCT command.
Contact Compliance (1/STIF)	Appears when Normal Stiffness Model Type is set to Constant Compliance.Sets the compliance factor, which is the reciprocal of the stiffness. This is a single-value adjustment.
Specify Field	Appears when Normal Stiffness Model Type is set to Nonlinear Stiffness.Sets the field or table that defines a nonlinear function that limits the depth of penetration when pressure increases. This option allows you to vary the stiffnesses by using multiple values. For example, you can vary the stiffness by starting with a soft value and then increasing the stiffness based on the distance between the contacting bodies.When you define the field, the label updates to Penalty Function (NPEN).For more information, see the NPEN parameter of the Samcef .MCT command.
Scale Factor	Appears when Normal Stiffness Model Type is set to Nonlinear Stiffness.Sets the scale factor for the nonlinear Penalty Function (NPEN) function that limits the depth of penetration when pressure increases.
Material	Appears when Normal Stiffness Model Type is set to Stiffness from Material.Specifies the material whose stiffness is taken into account in the stiffness computationSelect a material from the list, or click Choose Material to open the Material List dialog box where you can select the material.

Tangential Behavior page

Friction Coefficient (CF)	Lets you define the friction coefficient.For more information, see the CF parameter of the Samcef .MCT command.
Friction Type (OPFR)	Appears when Solution Applicability View is set to Nonlinear Analysis and Iteration Method is set to Coupled.NoNo friction at all.ClassicalClassical friction algorithm.InfiniteInfinite friction. The value of the Friction Coefficient is ignored.Function of VelocityThe friction coefficient depends on the relative velocity.For more information, see the OPFR parameter of the Samcef .MCT command.
Improve Convergence	Appears when Friction Type (OPFR) is set to Classical.Lets you enter a friction stiffness and sliding direction (3D elements) to help your model converge.Clear this check box to enable the default convergence algorithm.
Friction Stiffness (STFR)	Appears when the Improve Convergence check box is selected.Lets you define the friction stiffness between the friction stress and the relative displacement. The friction occurs along the Sliding Direction.For more information, see the Samcef .MCT command.
Sliding Direction (3D only) (FRM1)	Appears when the Improve Convergence check box is selected.Specifies the type of coordinate system for setting the sliding direction. The coordinate system definition is only suitable for target 3D element faces.For more information, see the Samcef .MCT command.
Local	Appears when Improve Convergence is selected.Lets you define the sliding direction for the friction .Click CSYS Dialog to use the CSYS dialog box to create the coordinate system, or click the list to choose a coordinate system command to create it.
Regularization Parameter (TOL)	Appears when Friction Type (OPFR) is set to Function of Velocity.Sets the value to use as the regularized friction coefficient as a function of the sliding velocity. This option applies to most sliding problems. For more information, see the Samcef .MCT command.

Damping page

Appears when Solution Applicability View is set to Nonlinear Analysis and Iteration Method is set to Coupled.

Damping
Damping Model Type	Specifies the damping model to apply.No DampingNo damping is applied.Normal DampingApplies the damping in the normal direction.Tangential DampingApplies the damping in the tangential direction.Normal and Tangential DampingApplies the damping in both the normal and tangential direction.For more information, see the Samcef .MCT command.
Normal Behavior
Appears when Damping Model Type is set to Normal Damping or Normal and Tangential Damping.
Specify Field	Sets the normal velocity coefficient. The value you enter specifies a table whose quantities are pressure divided by velocity. When you define the field, the label updates to Damping Function (UN1).
Scale Factor	Sets the scaling of the normal velocity coefficient.
Tangential Behavior
Appears when Damping Model Type is set to Tangential Damping or Normal and Tangential Damping.
Specify Field	Sets the tangential sliding velocity coefficient. The value you enter specifies a table whose quantities are pressure divided by velocity. The value of the table is then multiplied by the tangential sliding velocity to produce a tangential viscous pressure.When you define the field, the label updates to Tangential Damping Function (UN4).
Scale Factor	Sets the scaling of the tangential sliding velocity coefficient.

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Contact Parameters dialog box (Simcenter Samcef), Simcenter 3D 2021.1 Series

© 2020 Siemens

window.mainLanguage="en_US"

window.delivId=""

window.projectId=""

MathJax.Hub.Config({ TeX: { extensions: ["autoload-all.js"] }, tex2jax: { displayMath: [ ] }, "SVG": { scale: 125 } });