Beam Beam Contact Parameters dialog box (Simcenter Samcef)

Use this dialog box to create a Beam Beam 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 Beam Beam 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 OncePerform 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 NLIM, UN2 parameters of the Samcef .MCT LINE 1 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 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 LINE 1 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.
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 LINE 1 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 LINE 1 command.

Initial Penetration page

Option

Description

Offset of the Beam (DMIN)

Lets you define the distance offset.If the offset is positive, the computed distance between the Source Region nodes and the Target Region should be kept greater than the offset: this simulates an external contact between two cables.If the offset is negative, the computed distance between the Source Region nodes and the Target Region should be kept smaller than the absolute value of the offset. That means that the Source Region nodes are inside the Target Region: this simulates a cable that is moving inside another one.Note: The offset cannot be zero.For more information, see the DMIN parameter of the Samcef .MCT LINE 1 command.

Normal Behavior page

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

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.Constant StiffnessUses a basic method that allows you to adjust the contact stiffness by a single value.Nonlinear StiffnessLets you enter the 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.
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 LINE 1 command.
Specify Field	Appears when Normal Stiffness Model Type is set to Nonlinear Stiffness.Sets the field or table that defines the 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 LINE 1 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.

Tangential Behavior page

Friction Coefficient (CF)	Lets you define the friction coefficient.For more information, see the CF parameter of the Samcef .MCT LINE 1 command.
Friction Type (OPFR)	Appears when Solution Applicability View is set to Nonlinear Analysis and Iteration Method is set to Coupled.Specifies the type of friction.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 LINE 1 command.
Improve Convergence	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 LINE 1 command.
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 LINE 1 command.

Damping page

Appears when Solution Applicability View is set to All Solutions or 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.For more information, see the Samcef .MCT command.
Normal Behavior
Appears when Damping Model Type is set to Normal 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).For more information, see the Samcef .MCT LINE 1 command.
Scale Factor	Sets the scaling of the normal velocity coefficient.

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Beam Beam 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 } });