Segments (Loads and Constraints) Reference

Segments Manager Properties

Segments

Displays the number of segments that you created for a region (read-only).

Segments Manager Right-Click Actions

Create Segment

Adds a segment under the Segments node. You can choose between three classes of segments:

• Surface Segment—allows you to apply a load or constraint on part surfaces.
• Curve Segment—allows you to apply a load or constraint on part curves. This option is not compatible with the Thin Mesher, as this mesher does not preserve edges from part curves.
• Point Segment—allows you to apply a load or constraint on part points.

For a solid region, you can create as many segments as required by your analysis.

New Group

Allows you to organize the segments into groups. This option adds a node, [New Group], under the Segments node. You can move segments to groups using drag-and-drop. To move the segments back to their original location and delete a group, right-click the group node and select Ungroup.

Group By

Organizes the segments into subfolders, based on specified criteria:

• Physics Conditions —groups the segments that share the same physics conditions into a group.
• Physics Values—groups the segments that share the same physics values into a group.
• Class —groups the segments by class (surface, curve, or point).
• Surfaces—groups the segments based on the associated part surfaces.
• Curves—groups the segments based on the associated part curves.
• Points—groups the segments based on the associated part points.
• Type —groups the segments by type (load or constraint).

Segment Properties

Index

Specifies the unique number that identifies a segment (read-only).

Active

When deactivated, Simcenter STAR-CCM+ deactivates the segment. You cannot change the settings of deactivated segments. For grouped segments, the Active property on the [Group] node controls the status of the entire group.

Surfaces

Available for surface segments, specifies the part surfaces where the load, or constraint, is applied.

Curves

Available for curve segments, specifies the part curves where the load, or constraint, is applied.

Points

Available for point segments, specifies the part points where the load, or constraint, is applied.

Type

Specifies whether the segment represents a load or constraint condition.

Property Value	Activates
Load Allows you to apply a load on the selected Surfaces, Curves, or Points.	Solid Stress Loads See Solid Stress Loads.
Constraint Allows you to apply a constraint on the selected Surfaces, Curves, or Points.	Solid Stress Constraints See Solid Stress Constraints.

Segment Conditions and Values

You define loads and constraints by setting the physics conditions and values for the segments.

Solid Stress Load

Specifies the type of load that is applied to the part entities selected for the segment. You can specify force, pressure, and traction on surfaces, force and line load (force per unit length) on curves, and nodal force on points. When you define a surface or curve load, Simcenter STAR-CCM+ obtains the corresponding nodal forces by integrating the load over each element face, or edge, that lies on the surfaces or curves selected for the segment, using appropriate shape functions. When you define a point load, Simcenter STAR-CCM+ directly applies the nodal force on the part points assigned to the segment.

Method	Activated Values and Conditions
Force Available for surface, curve, and point segments. Specifies the load as a force field.	Force Set as a vector with a choice of coordinate system. Surface Segment: Simcenter STAR-CCM+ converts the specified force vector to a uniform surface traction. You are advised to specify the force using the Constant method. Use other methods with care. To convert the specified force to a surface traction, Simcenter STAR-CCM+ divides the force by the total area of all the surfaces that are assigned to the segment. The calculated traction is applied uniformly to each surface regardless of the local orientation of the surface. The applied load, that is, the sum of the nodal loads as specified for the segment, is not exactly equal to the sum of the forces that are derived for example from field functions or tabular data. In particular, force is not the nodal load applied to all the nodes on the surface. Curve Segment: Simcenter STAR-CCM+ converts the specified force vector into a uniform line load (force per unit length) across the curve segment. You are advised to specify the force using the Constant method. Point Segment: Simcenter STAR-CCM+ applies the specified force at each point of the specified part points.
Pressure Available for surface segments. Specifies the load as a pressure field, that is equivalent to specify the normal component of a surface traction with tangential components equal to zero.	Surface Load Linearization Available when the Nonlinear Geometry model is active in the solid physics continuum. See Nonlinear Geometry Model Reference. Surface Load Treatment Option Specifies how pressure and traction fields are treated at the solid element faces. Set this option only when the fields are spatially varying across the surfaces of the segment, that is, when you are specifying the pressure/traction profiles with a Method other than Constant. The available options are: Continuous—treats the pressure/traction fields as continuous functions across edges and vertices of neighbor elements. Discontinuous—treats the pressure/traction fields as constant over the element face, with field values computed at the face centroid. For constant pressure/traction profiles, the Continuous and Discontinuous options are equivalent. Pressure Set as a scalar field. Pressure loads are applied in the direction normal to the surface. Positive values correspond to compressive loads, whereas negative values correspond to tensile loads.
Traction Available for surface segments. Specifies the load as a traction field.	Surface Load Linearization Available when the Nonlinear Geometry model is active in the solid physics continuum. See Surface Load Linearization. Surface Load Treatment Option See Surface Load Treatment Option. Traction Set as a vector with a choice of coordinate system.
Line Load Available for curve segments. Specifies the load as a force per unit length.	Line Load Force per unit length, set as a vector with a choice of coordinate system.

Solid Stress Constraints

Specifies the type of constraint that is applied to the part entities selected for the segment. Simcenter STAR-CCM+ applies the constraint at each mesh node that lies on the part entities (either surfaces, curves, or points) selected for the segment.

To prevent conflict, do not prescribe a nonzero normal displacement on part surfaces that are associated with symmetry boundaries. See Symmetry Plane.

These options, applicable to solid elements, do not specify rotations.

Method	Corresponding Physics Value Nodes
Fixed Available for surface, curve, and point segments. Sets the components of the displacement field to zero, preventing the corresponding part surfaces, or part points, from moving in any direction.	None
Displacement Available for surface, curve, and point segments. Allows you to specify the components of the displacement field. If the values of all components are set to zero, this method is equivalent to the Fixed method.	Displacement Set as a vector with a choice of coordinate system. You can use the Composite method to select the components that you wish to constrain (use the properties of the Displacement > Composite node). All other methods constrain all the components.
Normal Displacement Available for surface segments. Allows you to specify the displacement field component in the direction normal to the selected part surfaces. Setting the normal displacement to zero prevents the part surfaces from moving in the normal direction. The normal displacement constraint is intended for plane surfaces or cylindrical surfaces, and it is not recommended on arbitrarily curved surfaces. The normal displacement option with single precision geometry may introduce tiny bumps in a plane surface, causing artificial stress concentrations. In general, you are advised to use the Displacement option with the Composite method, and fix the normal component of the displacement. If the surface is not aligned with the laboratory coordinate system, define an appropriate local coordinate system.	Normal Displacement Set as a scalar field. The displacement is applied in the direction normal to the surface. Positive values produce a tensile reaction, whereas negative values produce a compressive reaction.
Rigid Contact Available for surface segments. Accounts for the contact between the solid surface and a rigid obstacle. This type of constraint allows for frictionless contacts with rigid flat or curved surfaces.	Contact Gap Offset Allows you to specify an additional offset to the geometric contact gap between the solid surface and a rigid obstacle. Positive values increase the contact gap, whereas negative values decrease it. Activates additional physics conditions: Contact Constraint Enforcement Contact Linearization Contact Type Rigid Contact Obstacle
Lock current deformation Available for surface, curve, and point segments. Allows you to lock the displacement of the specified part entities to the current value. If you activate this setting at any stage, the simulation continues without further deformation of the specified part entities. Clearing the solution resets all part entities to their initial configuration.	None

Contact Constraint Enforcement

Available when the Solid Stress Constraints condition is set to Rigid Contact.

Method	Corresponding Physics Value Nodes
Penalty Allows you to relax the stiffness of the contact by allowing nonphysical penetrations of the solid into the obstacle. See Penalty Method for Contact Enforcement.	Penalty Contact Enforcement Allows you to specify the penalty parameter that relaxes the stiffness of the contact. Small values lead to larger, nonphysical penetrations of the solid into the plane. For infinitely rigid contacts, the penalty parameter approaches infinity. However, large values can cause convergence issues. For guidelines on how to estimate appropriate values for the penalty parameter, see Penalty Method for Contact Enforcement.
Augmented Lagrangian (Uzawa algorithm) Appropriate for simulations with a large penalty parameter and convergence issues. The Uzawa algorithm extends the penalty method with the Lagrange Multiplier Method (See Uzawa Algorithm for Contact Enforcement). Requires the Mortar Contact Discretization.	Penalty Contact Enforcement Allows you to specify the penalty parameter settings used in the Uzawa Augmentation. The available properties are: Penalty Parameter—defines the initial penalty parameter used during the Uzawa augmentation of the contact pressure. Penalty Parameter Update—allows Simcenter STAR-CCM+ to update the penalty parameter during each Uzawa Augmentation step using the conditions defined in Eqn. (4494). By updating the penalty parameter you can speed up the convergence of your simulation. Penalty Parameter Upper Bound—defines the maximum value of the penalty parameter. The penalty parameter is not updated further once this value is reached. Current Penalty Parameter—displays the current penalty parameter used during the Uzawa Augmentation.

Contact Discretization

Allows you to define the method for computing the virtual work for contact between a solid surface and a rigid obstacle (see Discretization of the Rigid Contact Gap).

• QPTS—computes the virtual work numerically using the Quadrature Point to Surface approach in combination with the penalty method (see Eqn. (4498)).
• Mortar—produces a finite element discretization of the contact pressure to express the nodal contact pressure as a function of the discretized contact gap. This is achieved by projecting the contact gap to the discretized contact pressure (see Eqn. (4502)).

If the QPTS method leads to poor convergence, use the Mortar method. The Mortar discretization method can improve convergence by ensuring that the number of contact constraints matches the number of contact degrees of freedom. However, the computational time per iteration increases compared to the QPTS method.

Contact Linearization

Available when the Solid Stress Constraints condition is set to Rigid Contact. When activated, affects the convergence of simulations containing rigid surfaces. The available settings are:

• Complete—linearizes the contact to achieve quadratic convergence, potentially at the expense of robustness.
• Partial—performs an incomplete linearization of the contact to achieve linear convergence. The simulation is more robust.

The curvature of the contact surface influences the closest point projection. If these influences are not accounted then for the resulting tangent matrix will be incomplete and result in linear convergence. To achieve a quadratic convergence the contact surface curvature is accounted for and the contact contribution to the tangent matrix will be the consistent linearization of the contact residual.

Contact Type

Available when the Solid Stress Constraints condition is set to Rigid Contact. Automatically set to Frictionless.

Rigid Contact Obstacle

Available when the Solid Stress Constraints condition is set to Rigid Contact.

Method	Corresponding Physics Value Nodes
Plane The rigid obstacle is an infinite plane.	Rigid Contact Plane Allows you to define the plane obstacle by specifying its origin and surface normal with respect to a coordinate system.
Cylinder The rigid obstacle is a solid or hollow cylinder whose cross-sectional shape can be either circular or elliptical.	Rigid Contact Cylinder Allows you to define the cylindrical obstacle by specifying its cross section and radius with respect to a coordinate system.
Tessellated Geometry Parts The rigid obstacle is a geometry part.	Tessellated Geometry Parts Allows you to define the geometry parts whose tessellated surfaces form the rigid obstacle surface. For the selected parts, you can also specify rigid motion. The available properties are: Tessellated Geometry Parts—Specifies the geometry parts. You can select shape parts or CAD parts that do not belong to the solid region or to imported CAE models. The tessellated surfaces of the selected parts must be closed. If you select shell parts, specify the orientation such that the front surface of the shell faces the solid region. As tessellated surfaces are comprised of flat triangles, quadrilateral elements of the rigid contact surface are divided into two triangular facets. Rigid Motion—defines the displacement of the contact obstacle using a rigid motion. The rigid motion is only taken into account in the contact computation and does not affect the Latest Surface representation.