9.6.3.1. Scope Settings

The properties for the Scope category are described in the following table. Also make sure you review the Stiffness Behavior Support Specifications topic at the end of the section.

Property	Description/Selections
Scoping Method	Specifies whether the Contact Region is applied to a Geometry Selection (default), a Named Selection, or to a Pre-Generated Interface for fracture mechanics (Interface Delamination) when you are using the Ansys Composite PrepPost (ACP) application.
Interface	This property displays when you select Pre-Generated Interface as the Scoping Method. It provides a drop-down list of the available interface layers that were imported from ACP.
Contact	Displays/selects which geometries (bodies, faces, edges, or vertices) or mesh entities (elements [3D shell only], element faces or node set) are considered in contact. The geometries can be manually selected or automatically generated. Important: Note the following requirements when scoping with mesh nodes. Can only be performed using manual scoping (no automatic detection). Is not supported in combination with the Shell Thickness Effect property (see below). For Face/Edge or Body/Edge contact, the edge must be designated as Contact. Body scoping always includes all pertinent faces in the solution process. A contact pair can have a flexible-rigid scoping, but the flexible side of the pair must always be the Contact side. If the Contact side of the contact pair is scoped to multiple bodies, all of the bodies must have the same Stiffness Behavior, either Rigid or Flexible. Note: When the Rigid Body Mesh Behavior is set to Dimensionally Reduced, the Contact scoping can not be scoped to a Named Selection of Mesh Entities.
Target	Displays which body element (body, face, or edge) or mesh entities (elements [3D shell only] or element faces) is considered Target (versus Contact). This element can be manually set or automatically generated. For Face/Edge or Body/Edge contact, the face or body must be designated as Target. Body scoping includes all pertinent faces in the solution process. If the Contact side of the contact pair has a flexible Stiffness Behavior then the Target side can be rigid. Multiple rigid bodies cannot be selected for the Target side scoping of the contact pair. The selection of multiple rigid bodies for the Target invalidates the Contact Region object and an error message is generated following the solution process. Note: If you click this field, the bodies are highlighted. Note: When the Rigid Body Mesh Behavior is set to Dimensionally Reduced, the Target scoping can not be scoped to a Named Selection of Mesh Entities.
Shared Target Body	This property displays when the Target is scoped to either edges or faces that are shared by more than one body and: The Contact or Target property is scoped to edges or faces that are shared by the scoping of a General Axisymmetric object. Or… When the Contact and Target properties are scoped to the edges and the Edge Contact Type property is set to Nodes on Edge. When displayed, this property provides a drop-down list that includes the bodies that share the edge or face. Scoping the property to one of these body selections specifies that the target elements are generated on top of elements of the selected body and their normal is outward to the boundary of the body.
Reverse Shared Contact Normal	Reverse Shared Contact Normal: This property displays when the Contact property scoping of the contact condition includes the following: One or more 2D edges, shared by more than one body, and that are not specified by a General Axisymmetric object. The Target scoping cannot be specified by a General Axisymmetric object, either. One or more 3D faces that are shared by more than one body. When displayed, you select subset of shared contact edges or faces to reverse the direction of the normal for the generated contact elements. Important: If a shared face is shared by both shell and solid bodies, the Reverse Shared Contact Normal property only displays when Contact Shell Face property is set to Top or Bottom. Note: You can set the Element Normals property of the Display category to Yes to display the normal directions of the elements in contact.
Reverse Shared Target Normal	Reverse Shared Target Normal: This property displays when the Target property scoping of the contact condition includes the following: One or more 2D edges, shared by more than one body, and that are not specified by a General Axisymmetric object. The Contact scoping cannot be specified by a General Axisymmetric object, either. One or more 3D faces that are shared by more than one body. When displayed, you select subset of shared target edges or faces to reverse the direction of the normal for the generated target elements. Important: If a shared face is shared by both shell and solid bodies, the Reverse Shared Target Normal property only displays when Target Shell Face property is set to Top or Bottom. Note: You can set the Element Normals property of the Display category to Yes to display the normal directions of the elements in contact.
Contact Bodies	This read-only property displays the name of the parts included in the Contact side of the Contact Region.
Target Bodies	This read-only property displays the name of the parts included in the Target side of the Contact Region.
Edge Contact Type	This property is visible when the Contact geometry is an Edge (of a line, shell, or solid body) and the Target geometry is an Edge, Face, or Element Face (of a shell or solid body). Property options include: Program Controlled (default): For 3D Structural analyses, the application internally uses the Line Segments (CONTA177 element) option. For all other cases, the application uses the Nodes on Edge (CONTA175 element) option as the internal setting. Exception: If you are performing a substructure analysis, or if your analysis is linked to a downstream Structural Optimization analysis (Future Analysis property set to Structural Optimization), then the application uses the CONTA175 element. Nodes On Edge: When selected, the application uses the CONTA175 element for the Contact Region. Line Segments: This option is only supported for structural physics-based analyses. When selected, the application uses the CONTA177 element for the Contact Region. Note: This property is not supported for contact between the edges of two line bodies.
Line-Line Detection	The application displays this property when you: Specifying beam edges as the scoping for both the Contact and Target properties. Or... Specify the Contact property as an edge (of a line, shell, or solid body) and the Target property an edge, face, or element face (of a shell or solid body) and the Edge Contact Type property set to Line Segments and the Formulation property is set to Augmented Lagrange or Pure Penalty. Property options include: External - Only 1 Segment External - Up to 4 Segments (default) External - Up to 8 Segments Internal Pipe Contact (only visible for beam-to-beam edge contact) Note: The external options enable you to specify the maximum number of target segments interacting with each contact detection point simultaneously. The Internal Pipe Contact can be used to model a beam (or pipe) sliding inside another hollow beam (or pipe). However, if the inner beam is much stiffer than the outer beam, the inner beam can be the target surface. This setting specifies a maximum of four target segments for the Contact edge (CONTA177). See the CONTA177 and 3D Beam-To-Beam Contact sections for additional technical details about this property.
Beam-Beam Model	The application displays this property when it detects beam-to-beam contact. It enables you to specify the contact traction-based model the application uses for Beam-to-Beam contact. Options include: Exclude Crossing Beams: For this option, the application excludes the contact for any beams that cross one another. The Mechanical APDL Reference for this option is KEYOPT(3) = 1. Only Crossing Beams: For this option, the application includes only the contact for beams that cross one another. The Mechanical APDL Reference for this option is KEYOPT(3) = 3. All (default): This is the default setting. The application includes all beam contact scenarios, which are: beam/edge to surface contact, parallel beam-to-beam contact, and crossing beam-to-beam contact. The Mechanical APDL Reference for this option is KEYOPT(3) = 2. For additional Mechanical APDL specific information, see KEYOPT(3) in the Mechanical APDL Contact Technology Guide.
Protected	Specifies if the contact entities (faces, edges, and vertices) are protected topology. Set the property to Yes to respect the geometry features the Contact is scoped to and ensure proper association between the geometry and mesh. Set the property to No to indicate that the topology may not be protected.
Contact Shell Face	Specifies whether the Contact should be applied on a surface body’s top face or bottom face. When scoped to an element face, the contact is applied to the scoped side (top/bottom) of the shell face. If you set Contact Shell Face to the default option, Program Controlled, then the Target Shell Face option must also be set to Program Controlled. The Program Controlled default option is not valid for nonlinear contact types. This option displays only when you scope a surface body to Contact Bodies.
Target Shell Face	Specifies whether the Target should be applied on a surface body’s top face or bottom face. When scoped to an element face, the target is applied to the scoped side (top/bottom) of the shell face. If you set Target Shell Face to the default option, Program Controlled, then the Contact Shell Face option must also be set to Program Controlled. The Program Controlled default option is not valid for nonlinear contact types. This option displays only when you scope a surface body to Target Bodies.
Shell Thickness Effect (See notes below as well as Using KEYOPT(11))	This property appears when the scoping of the contact or target includes a Surface Body. Options include: Yes: Include the property. No (default): Exclude the property. When set to Yes, the contact object becomes under-defined if the Offset Type of any scoped surface body is set to a value other than Middle. In this situation, the following error message will be displayed: "The shell thickness effect of a contact pair is turned on; however, the offset type of a shell body in contact is set to other than Middle. Set its offset type to Middle." In the presence of a Thickness, Imported Thickness, Layered Section, or an Imported Layered Section object, the following warning message will be issued if a solve is requested: "The shell thickness effect of a contact pair is turned on. Make sure that the offset type of the thickness, imported thickness, layered sections and imported layered sections objects associated with the shell bodies in contact are set to Middle."

Shell Thickness Effect

The Shell Thickness Effect allows users to automatically include the thickness of the surface body during contact calculations. Instead of contact being detected on the face of the surface body, contact will be detected a distance of half the thickness away from the face.

If the surface body undergoes large strains and changes thickness, the updated (current) thickness is also used in the contact calculations. However, to be able to take advantage of this feature, the Offset Type must be set to Middle.

For cases where Offset Type is set to Top or Bottom, you can do the following:

For a given contact region, if contact is occurring on the same face (Top or Bottom) as the offset, no special settings are required. The location of the nodes and elements of the surface body represent the actual position of that face.
For Rough, Frictionless, or Frictional contact types, if contact is occurring on the opposite face as the offset, specify a contact Offset equal to the shell thickness for the Interface Treatment. Note that changes in shell thickness for large strain analyses will not be considered.

Note: If the Shell Thickness Effect is activated, and you have specified a contact Offset for the Interface Treatment, the total offset will be half the thickness of the surface body plus the defined contact offset.

Postprocessing surface bodies using the Shell Thickness Effect has the following special considerations:

Because contact is detected half of the thickness from the middle of the surface body, viewing surface body results without Thick Shell and Beam (See the Style group of the Display tab) effects turned on will show an apparent gap between contact bodies. This is normal since contact is being detected away from the location of the nodes and elements.
When using the Contact Tool to postprocess penetration or gaps, these values are measured from the middle of the surface bodies (location of the nodes and elements), regardless of whether or not the shell thickness effect is active.

Stiffness Behavior Support Specifications

Note:

All geometric entities selected for a contact condition, on either the Contact or the Target side of the contact pair, must have the same setting for the Stiffness Behavior property.
If the Stiffness Behavior property of a geometry is set to Rigid, you must set the Definition property to Asymmetric.
You cannot scope the Target side in a contact pair to more than one rigid body.
If you have both rigid and flexible bodies in your contact pair, you must scope the rigid body as a Target.
For the Mechanical APDL solver, you cannot scope the Target side in a contact pair to the edge of a rigid body.