Region dialog box

If you are defining a rotor region, see Region (Rotor) dialog box (Simcenter Nastran).

Type (Simcenter Nastran only)
Region type list	Specifies the type of region to create:Edge Region lets you define a collection of edges to use as a source or target region. For example, you can use an Edge Region to define the Source Region in an Edge-to-Surface Gluing definition.Surface Region lets you define a collection of surfaces to use as the Source Region or Target Region in boundary conditions, such as contact and glue definitions.AML Region lets you define a collection of fluid faces to use as the Automatically Matched Layer Surface.Infinite Plane Region lets you select a collection of fluid faces to specify the location of an infinite plane with Rigid Plane (Symmetry, Zero Velocity) or Pressure Release Plane (Anti-Symmetry, Zero Pressure) boundary conditions.Rotor Region lets you define a rotor, bearing supports for the rotor, and define rotor-specific parameters for the rotor. For more information, see Region (Rotor) dialog box (Simcenter Nastran).Structural Surface Region on 2D Elements and 3D Element Faces lets you select 2D and 3D element faces to use as Structural Free-Faces for a Vibro-Acoustic Transfer Vector Output Request.Note: For these element faces, the software will export BSURF and BSURFS bulk entries, where each bulk entry has a unique identifier.Duct Inlet Region lets you define the properties for a duct mode inlet. Duct Outlet Region lets you define the properties for an anechoic end duct.
Type (Multiphysics only)
Region type list	Specifies the type of region to create:Edge Region lets you define a collection of edges to use as a source or target region in boundary conditions, such as contact and glue definitions.Surface Region lets you define a collection of surfaces to use as source or target region in boundary conditions, such as contact and glue definitions.Void Region lets you define a collection of faces or edges with specified pressure and heat transfer characteristics that you use in the Thermal Void loads. For more information, see Region (Void) dialog box (Thermal/Flow/ESC/Multiphysics).
Type (Thermal/Flow, Electronic Systems Cooling, and Space Systems Thermal only)
Region type list	Specifies the type of region to create:Region lets you define a collection of elements, element edges, element faces, polygon edges, and polygon faces to use as a primary or secondary region in manual pairing in the Disjoint Fluid Mesh Pairing or Surface-to-Surface Contact simulation object.Surface Region lets you define a collection of surfaces that represent the printed circuit board in the Printed Circuit Board and PCB Component simulation objects.Void Region lets you define a collection of faces or edges with specified pressure and heat transfer characteristics that you use in the Thermal Void loads. For more information, see Region (Void) dialog box (Thermal/Flow/ESC/Multiphysics).
Type (Samcef only)
Region type list	Specifies the type of region to create. For instance:Edge Region lets you define a collection of edges to use as a Source Region or Target Region in contact and glue conditions.Surface Region lets you define a collection of surfaces to use as the Target Region of a Rigid-Flexible Contact condition.
Type (LS-DYNA only)
Region type list	Cross-Section Region lets you define a cross section comprised of
Name
Name	Sets the name for the region.
Label	Sets a unique numerical identifier for the region.
Region Objects
Group Reference	Lets you use a group to define a region. For more information, see Group Reference options.
Select Object	Lets you select the edges, faces, elements, or nodes to define a new region. The type of objects you can select depends upon your selected solver.
Stacked Smart Selector Methods	Opens the Smart Selector Methods dialog box where you can specify a progression of smart selection filters.For more information, see Smart Selector Methods dialog box.
Select Associated Faces	Appears when the Region dialog box is being used to define edge-to-edge contact and the edge you select for the region is an internal edge.Lets you select the polygon face to associate with the edge selection.
Infinite Plane Type
Infinite Plane Type	Specifies the type of infinite plane that represents the boundary condition.Rigid Plane (Symmetry, Zero Velocity) — Represents a zero normal velocity (Vn=0).Use this type of plane to represent the acoustically reflective boundary. Reflection occurs when there is an impedance mismatch (that is, if the characteristic impedance of one region is significantly higher than the other region).An example of a rigid plane is a concrete surface (hard surface).Pressure Release Plane (Anti-Symmetry, Zero Pressure) — Represents a zero acoustic pressure (p=0) or a free surface.Use this type of plane to represent the acoustically reflective boundary between a fluid with higher characteristic acoustic impedance and a fluid with much lower impedance, with the reference domain of interest being the one with higher impedance.An example of a pressure release plane is the free surface of water to air above a submarine that radiates acoustic energy.Note: Acoustic boundary conditions are determined by how the acoustic fluid is supported at its boundaries.If a structure supports the acoustic fluid, such as the rigid walls of a tank, the acoustic boundary is a rigid plane or zero velocity condition.If no structure supports the acoustic fluid, such as the free surface of a fluid, the acoustic boundary is a pressure release or zero pressure condition. Examples include an air-to-water interface, or a large impedance mismatch between two fluids in the acoustic region.
Card Name	Displays the name of the corresponding solver command.

Simcenter Nastran Acoustics Duct region options

Shape
Shape	Specify the shape of your duct inlet or outlet as Circular, Annular, or Rectangular.The Show Shortcuts option gives you the option to select one of the three shapes using an icon selection.
Parameters (for Duct Inlet Region only)
Axis Offset Value	Allows you to optionally offset the inlet location of a duct mode inlet axially.
Transverse Axis	When Transverse Axis Automatically is selected, the software automatically determines the duct axis. You can manually define the duct axis by toggling off the automatic option, then specifying the vector.See the vector dialog box Vector dialog box.

Simcenter Nastran and Multiphysics contact options

Common Contact Parameters (BCRPARA)
Surface	For linear contact solutions (SOLs 101, 103, 111, and 112), indicates the contact side of 2D shell elements.Select Top to make the contact side consistent with the shell element normals.Select Bottom to make the contact side opposite of the shell element normals.For information on the use of the Surface option in advanced nonlinear solutions (SOL 601 and 701), see BCRPARA in the Simcenter Nastran Quick Reference Guide.
Offset	Defines the offset distance for the contact region. Use the Offset option to account for a rigid layer that might occur between two faces in contact.You can also use Offset to analyze an interference fit problem if unconnected elements are modeled as being coincident. For example, you can use Offset to represent the theoretical interference of those elements.Note: For advanced nonlinear solutions (SOL 601 and 701), this option is not valid if the specified Contact Algorithm for the Contact Set Parameters modeling object associated with this solution is set to Rigid Target. For more information, see Defining parameters for contact conditions (Simcenter Nastran).
Nonlinear Contact Parameters (BCRPARA)
Type	For advanced nonlinear solutions (SOL 601 and 701), indicates whether a 3D contact region is a rigid surface.Select Flex to indicate that the region is not rigid.Select Rigid to indicate that the region is rigid.For more information, see BCRPARA in the Simcenter Nastran Quick Reference Guide and Contact conditions in the Simcenter Nastran Advanced Nonlinear Solution—Theory and Modeling Guide.
Select Master Grid Point	If you select Rigid from the Type list, lets you select the node (master grid point) that controls the motion of the rigid surface. Rigid surfaces have no flexibility apart from their rigid body motions. Internally, the software uses rigid links to connect all the nodes on the rigid target region to this master node.

MSC Nastran options

Dimension	Specifies the dimension of the body in contact. Only the 3D option is supported. 3D bodies can be composed of rigid surfaces, shell elements, or solid elements.For more information, see BCBODY1 in the MSC Nastran Quick Reference Guide.
Behavior	Specifies the behavior of a surface. Only the DEFORM option is supported, which means that the body is deformable.For more information, see BCBODY1 in the MSC Nastran Quick Reference Guide.
Contact Body Parameters	Lets you specify the Contact Body Parameters modeling object that defines the structural and thermal properties of the contact body. The options in the Contact Body Parameters dialog box correspond to the fields on the BCBDPRP bulk data entry.For more information, see Defining contact parameters (MSC Nastran).

Abaqus options

Region Parameters
Trim	Controls the trimming of open free surfaces.Select Yes to invoke the trimming of open free surfaces.Select No to suppress surface trimming.
Surface Definition Type	Controls whether the software creates an element-based surface or a node-based surface.Select Element to create an element-based surface.Select Node to create a node-based surface.
Element Free Face	If you select Element from the Surface Definition Type list, controls whether Abaqus uses element free faces to create the element-based surface.
Side	Lets you define sides for an element-based surface. For an element-based surface (*SURFACE keyword), you can define a single-sided surface on the positive or negative face of structural, surface, or rigid elements.Select SPOS to specify that the face is the positive side in the element-based surface. The positive face is the face in the direction of the element normal.Select SNEG to specify that the face is the negative side in the element-based surface. The negative face is face in the direction opposite to the element normal. Before you use the Side option to designate the positive or negative side of a surface, you should first ensure that all of the specified elements have their normals oriented consistently.Tip: Use the 2D Element Normals command to evaluate the consistency of the element normals in the mesh.
*Reference Node and Type (RIGID BODY)
Type	Select Flex to indicate that the region is not rigid.Select Rigid to indicate that the region is rigid.
Select Master Grid Point	If you select Rigid from the Type list, lets you select the node (master grid point) that controls the motion of the rigid surface. Rigid surfaces have no flexibility apart from their rigid body motions. Use this option to rigidly link the nodal degrees of freedom of the nodes on the rigid surface to the selected master grid point.

ANSYS options

Parameters
Use ESURF	Controls when the software creates the ANSYS contact elements.Select Yes to have the software use the ANSYS ESURF command to automatically create the ANSYS contact elements.Select No to have the software create the ANSYS contact elements in your ANSYS input file when you export or solve your model. If you select this option, the software uses the CMBLOCK command to write out the group of nodes that define the region.For more information, see Creating ANSYS rigid bodies.
Correct direction of normals	Available if Use ESURF is set to Yes.For a region that is comprised of 2D elements, controls the direction of the normals on the contact elements that the software generates on the faces of those 2D elements.Select Top to have the software generate contact elements with normals that are the same as the normals of the underlying 2D elements.Select Bottom to the software generates contact elements with normals that are the opposite of the normals of the underlying 2D elements.Select Reverse to have the software reverse the normal direction for selected contact elements.For more information, see ESURF in the ANSYS Commands Reference.
Region Type and Pilot Node
Type	Lets you specify the type of region to create.Select Flexible to create a flexible region.Select Rigid to create a rigid region.For more information, see Creating ANSYS rigid bodies.
Select Master Grid Point	Available if Type is set to Rigid.Lets you designate a node to serve as the pilot node. During the contact analysis, ANSYS uses the motion of the pilot node to determine the motion of the rigid body.

LS-DYNA options (Cross-Section Region type)

Cutting Plane
Orientation	Lets you define the orientation of the plane to use as the cutting plane.Select Plane to select a plane to define the cutting plane.Select Point and Vector to specify a point and a vector to define the cutting plane.
Offset from Selected Point	Available if you select Point and Vector from the Orientation listLets you define a distance from which to offset the plane from the point that you select.
Specify Point	Available if you select Point and Vector from the Orientation listLets you specify a point that defines the origin of the cutting plane.
Specify Vector	Available if you select Point and Vector from the Orientation listLets you define a vector that defines the direction in which to create the cutting plane.
Specify Plane	Available if you select Plane from the Orientation listLets you select or create the plane to use as the cutting plane.
Physical Property Tables
Property	Lets you select one or more physical property tables from the Physical Property Table Manager dialog box to define the initial stress. The software applies the stress values to the meshes associated with those physical property tables.
Properties
Plane Type	Lets you specify the type of cutting plane to use to define the cross-section.Select Rectangular to define a rectangular shaped cutting plane.Select Circular to define a circular shaped cutting plane.
Specify Vector	Available if Plane Type is set to Rectangular.
Edge Length in L Direction	Available if Plane Type is set to Rectangular.Defines the length of edge a in the L direction.
Edge Length in M Direction	Available if Plane Type is set to Rectangular.Defines the length of edge b in the L direction.
Radius	Available if Plane Type is set to Circular.Defines the radius of a circular cutting plane.
Local System Type (ITYPE)	Controls how the software outputs the force resultants.Select Rigid Body to output force resultants in the updated local coordinate system of a rigid body that you specify.Select Local CSYS to output force resultants in a local coordinate system that you specify.
Rigid Body	Available if Local System Type (ITYPE) is set to Rigid Body. Lets you specify the ID (label) of the rigid body to use. The software outputs the force resultants in the local coordinate system of the rigid body you specify.
Coordinate System for Resultants	Available if Local System Type (ITYPE) is set to Local CSYS. Lets you specify a coordinate system to use to output the force resultants.

Learn more

Working with reusable regions

Look up more details

Automatically Matched Layer dialog box

Vibro-Acoustic Transfer Vector Output Request dialog box

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Region 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 } });