Products: ABAQUS/Standard ABAQUS/Explicit ABAQUS/CAE
In ABAQUS surfaces:
can be used to define contact and interactions, including acoustic-structural interactions;
can define regions used to prescribe distributed surface loads;
can be used to tie dissimilar meshes together;
can define cavities used for a cavity radiation analysis in ABAQUS/Standard;
can define pre-tensioned sections used in prescribing assembly loads in ABAQUS/Standard;
can define sections used for tracking the average motion of a surface in ABAQUS/Explicit;
can define sections for output quantities such as the total force transmitted through a surface;
are geometric entities that have an area associated with them but have zero volume;
have an identifiable orientation defined by their normals;
are defined by specifying nodes or node sets, an analytic curve or surface, or element faces, edges, or ends; and
can be deformable, rigid, or partially deformable and partially rigid.
Surfaces can be used to model the interaction of two or more distinct bodies in a mechanical, acoustic, coupled acoustic-structural, coupled thermal-mechanical, thermal, coupled thermal-electrical, or cavity radiation analysis. A rigid surface can be used to model a body that is much stiffer than the rest of the model in a mechanical or coupled thermal-mechanical analysis, but no heat can be transferred to the rigid body. In acoustic-structural analysis, surfaces can be used to define impedance boundary conditions, including first-order conditions for modeling acoustic radiation.
Surfaces can be used to define a region on which a distributed surface load is prescribed; this can facilitate user input of distributed surface loads for complex models. In addition, surfaces can be used to define multi-point or coupling constraints. Surfaces can also define pre-tension sections used in prescribing assembly loads in ABAQUS/Standard.
Finally, surfaces can be used to define sections to obtain output of accumulated quantities; this provides a “free body diagram” output, allowing analyses of “force-flow” through a statically indeterminate structure.
Three types of surfaces can be defined in ABAQUS:
Element-based surfaces are defined on the faces, edges, or ends of elements and are usually continuous. The elements can be deformable or rigid, leading to a surface that is deformable or rigid. When some of the deformable elements underlying a surface are part of a rigid body, the surface will become partially deformable and partially rigid.
In ABAQUS/Explicit a default element-based surface that includes all bodies in the model is provided for use with the general contact algorithm.
Node-based surfaces are defined on nodes and, hence, are by definition discontinuous. A user-defined area can be associated with each node on the surface.
Analytical surfaces are defined directly in geometric terms and are always rigid.
Element-based surfaces contain more intrinsic information than either node-based surfaces or analytical rigid surfaces. When an element-based surface is used in a mechanical contact analysis, ABAQUS can associate a surface area with each node and can calculate the contact stress acting on the surface. In contrast, ABAQUS may not be able to calculate accurate contact stresses when a node-based surface (“Defining node-based surfaces,” Section 2.3.3) is used because the actual area associated with each node may not be correct. In addition, when a surface formed by shell, membrane, or rigid elements is used, ABAQUS can consider the thickness and possibly the offset of the reference surface of these elements in some applications that refer to surfaces. For example, these thicknesses are accounted for by all contact algorithms available in ABAQUS/Explicit and by the surface-to-surface, small-sliding contact formulation in ABAQUS/Standard.
Contact between two node-based surfaces or a node-based surface with itself is not allowed; contact between two analytical rigid surfaces or an analytical rigid surface with itself is not allowed. Contact between two rigid surfaces defined using rigid elements is not allowed in ABAQUS/Standard and is allowed only with penalty contact in ABAQUS/Explicit.
Surface definitions cannot change from step to step; however, new surfaces can be defined upon restart.
In ABAQUS/CAE many modeling operations are performed by picking geometry with the mouse. For example, a contact pair can be defined by picking faces on geometric part instances. Each such face must be translated into a surface in the input file. Such a surface is assigned a name by ABAQUS/CAE and is marked as internal. These internal surfaces can be viewed using display groups in the Visualization module of ABAQUS/CAE (see Chapter 51, “Using display groups to display subsets of your model,” of the ABAQUS/CAE User's Manual).
| Input File Usage: | *SURFACE, NAME=surface_name, INTERNAL |
Refer to the subsequent sections on the different surface types available in ABAQUS for details on the general restrictions that apply to all surface definitions of a given type. In addition, some features in ABAQUS that use surfaces impose other restrictions on surface characteristics. These limitations are discussed in the following sections:
In models that are defined in terms of an assembly of part instances, all surfaces must belong to a part, part instance, or the assembly. All of the general restrictions on surfaces still apply in such models. Additional rules are given in “Defining an assembly,” Section 2.9.1.