Contact Parameters- Multi-Step Nonlinear Kinematics Pair dialog box

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
Description	Sets a description for this set of contact parameters.You can optionally click Description to open the Description dialog box. This lets you see more of the text that you type, as well as cut, copy, or paste text.This description appears only on this dialog box.
Card Name	Displays the name of the corresponding solver command or keyword.

General Parameters page

Option	Description
Contact Surfaces (NSIDE)	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.For more information, see the NSIDE parameter of the BCTPAR2 bulk entry.
Continuous Segment Normal (SEGNORM)	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.If your model has a curved target that is meshed with linear elements, the normal directions are discontinuous between elements. This leads to convergence problems. Use this option to obtain unity in the normal directions at nodes and to define smooth transition between facets of the target.Used for Single-Sided ContactThe continuous (interpolated) contact segment normal is used only for single-sided contact.UsedThe continuous (interpolated) contact segment normal is used. Smooth contact is allowed for both single-sided and double-sided contact. The effect is the same.Not UsedThe continuous (interpolated) contact segment normal, that is, smoothing, is not used. The contact occurs with element normal directions and element topology with no modifications. For more information, see the SEGNORM parameter of the BCTPAR2 bulk entry.
Contact Pair Status when the Simulation Starts (ACTIVE)	Defines the status of the contact at the start of the computation.Contact Pair Status when the Simulation Starts (ACTIVE) (Default)Activates the contact at the beginning of the subcase (time=0s). Initial penetrations are accounted for 100% at the start of the subcase. This is useful for modeling purposes, for example, when you want to set the load from the first subcase.Caution: This is the default value. The effect of this option is different depending on whether the first subcase contains contact. To avoid unexpected contact behavior, see Setting initial contact status in Enabling and disabling contact in subcases (SOL 402) to ensure that you understand its effect.Contact Pair Status when the Simulation Starts (ACTIVE) Activates the contact during the subcase. Penetration is ramped from 0% (at time=0s) to 100% (at the end of the subcase). This is useful when initial penetrations are too high, so you want to ramp them slowly.For more information, see the ACTIVE parameter of the BCTPAR2 bulk entry.
Displacement Formulation (DISP)	Specifies the displacement formulation, which determines whether contact conditions are updated. DefaultNo displacement formulation is selected, and the DISP bulk entry is not exported to the .dat file. In this case, the solver chooses the most appropriate default based on your value for Large Strains (PARAM,LGDISP).Small DisplacementContact 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.Large DisplacementContact 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.Note: The Large Displacement formulation requires that you enable large strains and/or large displacements by selecting the Large Strains and/or Large Displacements check boxes on the Solution dialog box, Parameters page. If these check boxes are cleared, the solver generates a fatal error.For more information, see the DISP parameter of the BCTPAR2 bulk entry.
Contact Regions Tying in Normal Direction (TIED)	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 TiedFor a contact condition that works only in compression. Most contact is not tied. TiedFor 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.Remains Tied After Contact is ActiveFor 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.For more information, see the TIED parameter of the BCTPAR2 bulk entry.
Contact Node Tying Tolerance (TIEDTOL)	Appears when Contact Regions Tying in Normal Direction (TIED) is set to Tied.Sets the tolerance that determines when the source (contactor) nodes are tied to the target region. If the distance between the source (contactor) node and the target region is less than or equal to this value, the contact pair is tied together.For more information, see the TIEDTOL parameter of the BCTPAR2 bulk entry.
Extension Factor (EXTFAC)	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.The default value depends on how you set Displacement Formulation (DISP):If Displacement Formulation (DISP) is set to Small Displacement, the Extension Factor (EXTFAC) default is 0.1If Displacement Formulation (DISP) is set to Large Displacement, the extension factor default is 0.025.For more information, see the EXTFAC parameter of the BCTPAR2 bulk entry.

Initial Penetration page

Option	Description
Initial Penetrations/Gaps (INIPENE)	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. Calculate from Geometry/Print Penetrating NodesContact 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 Penetrations to ZeroInitial 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 GAPVALInitial penetrations or gaps are overridden by the value for Contact Gap Distance (GAPVAL). Set Penetrations to Zero for the Closest NodePenetrations are reset to a new initial condition in which no interference exists for the closest node.Set Gap or Penetration for the Closest Node to an Interference of GAPVALGaps and penetrations are both reset to a new initial condition in which GAPVAL provides an interference for the closest node.For more information, see the INIPENE parameter of the BCTPAR2 bulk entry.
Contact Gap Distance (GAPVAL)	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 GAPVAL parameter of the BCTPAR2 bulk entry.
Penetration Depth (PDEPTH)	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 PDEPTH parameter of the BCTPAR2 bulk entry.
Default Offset Distance for Contact Regions (OFFSET)	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 OFFSET parameter of the BCTPAR2 bulk entry.
Shell Thickness and Z-Offset (SHLTHK)	Specifies whether thicknesses and Z-offsets of shells are included in the calculations of initial penetration of contacting surfaces of shells.IncludeThe software automatically includes the offset between the shell elements and the outer surfaces of the shells in the calculation. This method of automatically including the offset is useful when a group of shells contains elements with different thicknesses, or if computation of Contact Gap Distance (GAPVAL) for each contact is complicated. Use this option when:Contact involves shell elements and no Contact Gap Distance (GAPVAL) 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 (GAPVAL) for each contact is complicated.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 (GAPVAL), specified manually.For more information, see the SHLTHK parameter of the BCTPAR2 bulk entry.

Normal Behavior page

Option	Description
Normal Regularization Type	Specifies how you want the software to regularize the model. Normal regularization impacts convergence but not the results. 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.We recommend starting with Default unless you have contact between parts with very different stiffnesses. If your model has contact between parts with very different stiffness, try setting Normal Regularization Type to Automatic Choice.Computed from Contact SupportsUses 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.User DefinedUses the value you specify for Normal Regularization Value (PRCS).Automatic ChoiceAutomatically chooses between Characteristic Stiffness of the Whole Structure (-1) and Computed from Contact Supports (-2) depending on the relative stiffnesses of the two parts.Characteristic Stiffness of the Whole StructureSets Normal Regularization Value (PRCS) to -1. The software uses the characteristic stiffness of the whole structure.
Normal Regularization Value (PRCS)	Appears 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 NLCNTL2 bulk entry.
Normal Stiffness Model Type	Specifies the method for defining the contact stiffness. Contact stiffness can help the solver to converge because it allows the contact to penetrate and then releases the contact constraints. However, you should not use contact stiffness if the solution converges without it. Changing Normal Stiffness Model Type has an impact on both convergence and the results. Note: If you use a normal contact stiffness, you must check the contact penetration results and final separation distance. If the penetration is too high, the normal contact stiffness needs to be increased.To request the contact penetration results, in the Structural Output Requests dialog box, click the Contact Result page, select the Enable BCRESULTS Request check box, and from the Separation and Slide Distance list, select SEPDIS.DefaultUses hard contact, which is infinite stiffness. Select this option for fully rigid contact.We recommend starting with Default. In most cases, selecting Default is the best option. Constant StiffnessBasic method that allows you to adjust the contact stiffness by a single value.Constant ComplianceBasic method that allows you to adjust the contact stiffness by a single value, but setting an inverse of the stiffness. Nonlinear StiffnessNonlinear function 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. When you select this option, you set the function or table in Normal Behavior Penalty Function (NPENAL).Automatic ChoiceComputes a stiffness value from the stiffness of both contact supports, the average size of the contact target support, and based on the materials in contact. When you select this option, you must check to ensure that the results are consistent.Note: To view stiffness values in the .f06 file, search for MCT, and in the table with MCT numbers (Nastran numbers that identify the contact), look at the STIFFNESS columns.
Normal Contact Modulus (NCMOD)	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 NCMOD parameter of the BCTPAR2 bulk entry.
Constant Compliance Factor (CFACTOR1)	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. For more information, see the CFACTOR1 parameter of the BCTPAR2 bulk entry.
Normal Behavior Penalty Function (NPENAL2)	Appears when Normal Stiffness Model Type is set to Nonlinear Stiffness.Sets the function or table that describes the relationship between the normal distance and the contact pressure. 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.If you use a table field, the X-axis is contact pressure (positive unit of pressure or force per distance squared) and the Y-axis is contact penetration distance (negative unit of length).For more information, see the NPENAL2 parameter of the BCTPAR2 bulk entry.

Tangential Behavior page

Option	Description
Friction Model Type (FRICMOD)	Specifies the type of friction model that determines how to handle complicated friction effects, such as friction between two different surface materials, or between two surfaces that have lubrication. BCTSET ConstantUses the Coefficient of Static Friction (FRICi) value that you set in the Surface-to-Surface Contact dialog box.Advanced Tables EvolutionComputes the friction coefficient as the product of the constant friction value defined by Friction Coefficient 1 (FPARA1) and existing functions depending on time (CFNF), temperature (CFTE), or velocity (CFVE). InfiniteUses an infinite friction coefficient. When you select this option, all of the friction parameters (BCTPAR2) are ignored, including the value for BCTSET Constant.Static/Dynamic CoefficientsUses two friction coefficients, depending on the sliding velocity. Static friction coefficient Friction Coefficient 1 (FPARA1) at low sliding velocity Dynamic friction coefficient Friction Coefficient 2 (FPARA2) at larger sliding velocity The low and high velocity are defined by the value you enter for Critical Sliding Velocity (VCRIT). The low sliding velocity is less than or equal to the value for VCRIT, and the high sliding velocity is greater than the value for VCRIT. When you select Static/Dynamic Coefficients, all other friction parameters are ignored, and the friction coefficient (FRICi) defined by Coefficient of Static Friction in the Surface-to-Surface Contact dialog box is ignored. Velocity Linear EvolutionUses a friction coefficient that varies linearly with the sliding velocity between the values for Friction Coefficient 1 (FPARA1) and Friction Coefficient 2 (FPARA2), up to the value that you set for Critical Sliding Velocity (VCRIT). After the friction coefficient reaches this value, it remains constant. Time Linear EvolutionUses a friction coefficient that varies linearly with time between the values for Friction Coefficient 1 (FPARA1) and Friction Coefficient 2 (FPARA2), up to the value that you set for Transition Time (TCRIT). After the friction coefficient reaches this value, it remains constant. When you select Time Linear Evolution, all other friction parameters are ignored, and the friction coefficient (FRICi) defined by Coefficient of Static Friction in the Surface-to-Surface Contact dialog box is ignored.
Friction Coefficient 1 (FPARA1)	Appears when Friction Model Type is set to Advanced Tables Evolution, Static/Dynamic Coefficients, Velocity Linear Evolution, or Time Linear Evolution.For more information, see the FPARA1 parameter of the BCTPAR2 bulk entry.
Friction Coefficient 2 (FPARA2)	Appears when Friction Model Type is set to Static/Dynamic Coefficients, Velocity Linear Evolution, or Time Linear Evolution.For more information, see the FPARA2 parameter of the BCTPAR2 bulk entry.
Critical Sliding Velocity (VCRIT)	Appears when Friction Model Type is set to Static/Dynamic Coefficients or Velocity Linear Evolution.For more information, see the VCRIT parameter of the BCTPAR2 bulk entry.
Friction Coefficient vs Sliding Velocity (CFVE)	Appears when Friction Model Type is set to Advanced Tables Evolution.For more information, see the CFVE parameter of the BCTPAR2 bulk entry.
Friction Coefficient vs Time (CFNF)	Appears when Friction Model Type is set to Advanced Tables Evolution.For more information, see the CFNF parameter of the BCTPAR2 bulk entry.
Friction Coefficient vs Temperature (CFTE)	Appears when Friction Model Type is set to Advanced Tables Evolution.For more information, see the CFTE parameter of the BCTPAR2 bulk entry.
Transition Time (TCRIT)	Appears when Friction Model Type is set to Time Linear Evolution.For more information, see the TCRIT parameter of the BCTPAR2 bulk entry.
Regularization Model Type	This regularization is for the tangential direction (friction). The regularization models ensure a smooth transition of friction stress between sliding and non-sliding regions, which aids in convergence. The regularization models are numerical, not physical.Specifies whether you want the regularization to be based on sliding velocity or displacement.DisplacementSmooths the transition when sliding changes direction. Note: If you select the Displacement regularization model type but omit a value for Stiffness Between Friction Stress and Relative Displacement (STFR), the software computes a default value. Sliding VelocitySmooths the transition when the velocity nears zero. When the sliding velocity is greater than or equal to the threshold you enter for Sliding Velocity (TOL), the regularization stops.No RegularizationDisables stiffness. This causes an abrupt transition between sticking and sliding, which is not recommended. Select this option when the contact does not require quick adjustments. However, regularization is typically recommended. Automatic Friction StiffnessUses a value that is computed from the stiffness of both contact supports and the average size of the contact target support.
Stiffness Between Friction Stress and Relative Displacement (STFR)	Appears when Regularization Model Type is set to No Regularization, Displacement, or Automatic Friction Stiffness.Sets the stiffness between the friction stress (also called tangential stress) and the relative displacement. Use this option to slow down sliding that is too quick because of reduced friction.To define the stiffness to use, enter a value greater than 0.0.For more information, see the STFR parameter of the BCTPAR2 bulk entry.
Sliding Velocity (TOL)	Appears when Regularization Model Type is set to Sliding 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 TOL parameter of the BCTPAR2 bulk entry.

Damping Models page

Option	Description
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.
Normal Velocity Coefficient (DPARA1)	Appears when Damping Model Type is set to Normal Damping or Normal and Tangential Damping.Sets the normal velocity coefficient. The value you enter specifies a table whose quantities are pressure divided by velocity. They are functions of the normal distance DPARA1=f(n).For more information, see the DPARA1 parameter of the BCTPAR2 bulk entry.
Tangential Velocity Coefficient (DPARA2)	Appears when Damping Model Type is set to Tangential Damping or Normal and Tangential Damping.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.For more information, see the DPARA2 parameter of the BCTPAR2 bulk entry.

Learn more

SOL 402 Multi-Step Nonlinear Kinematics

SOL 402 Multi-Step Nonlinear Kinematics workflow

Defining parameters for contact conditions (Simcenter Nastran)

Setting up contact (SOL 402)

Enabling and disabling contact in subcases (SOL 402)

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Contact Parameters- Multi-Step Nonlinear Kinematics Pair dialog box, 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 } });