Virtual Thread Parameters dialog box

Use this dialog box to create the Virtual Thread Parameters modeling object, which you can apply to a Virtual Thread Contact simulation 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
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
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 BVTPAR 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 BVTPAR bulk entry.
Contact Node Tying Tolerance (TIEDTOL)	Appears when Contact Regions Tying in Normal Direction (TIED) is set to TIED.Sets the tolerance for determining when contact nodes are tied to the target region. A contact node is tied to its target region if the distance between them is less than or equal to the value you set for this option.For more information, see the TIEDTOL parameter of the BVTPAR 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 BVTPAR bulk entry.

Initial Penetration page

Option	Description
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 BVTPAR 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.In most cases, selecting Default is the best option. 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 ChoiceSets Normal Regularization Value (PRCS) to -3.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.DefaultUses hard contact, which is infinite stiffness. Select this option for fully rigid contact. In most cases, selecting Default is the best option.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 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 ChoiceUses a value that is computed from the stiffness of both contact supports and the average size of the contact target support.
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 BVTPAR 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 BVTPAR 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 BVTPAR 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. BVTSET ConstantUses the Coefficient of Static Friction (FRICi) value that you set in the Virtual Thread 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 (BVTPAR) are ignored, including the value for BVTSET 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 Virtual Thread Contact dialog box is ignored.
Friction Coefficient 1 (FPARA1)	Appears when Friction Model Type is set to Advanced Tables Evolution or Time Linear Evolution.For more information, see the FPARA1 parameter of the BVTPAR bulk entry.
Friction Coefficient 2 (FPARA2)	Appears when Friction Model Type is set to Time Linear Evolution.For more information, see the FPARA2 parameter of the BVTPAR 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 BVTPAR 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 BVTPAR 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 BVTPAR 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 BVTPAR 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. 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 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 BVTPAR 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 BVTPAR 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 BVTPAR bulk entry.

Learn more

Modeling bolt threads (SOL 402)

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Virtual Thread Parameters 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 } });