Why Use Surfaces?
Surfaces can be used to model the interaction of two or more distinct bodies in a mechanical, acoustic, coupled acoustic-structural, coupled thermomechanical, coupled thermal-electrical-structural, thermal, coupled thermal-electrical, or cavity radiation analysis. A rigid surface can be used to represent a body that is much stiffer than the rest of the model in a mechanical or coupled thermomechanical analysis, with the limitation that 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.
The following types of surfaces can be defined in Abaqus:
Element-based surfaces are defined on the faces, edges, or ends of elements. 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.
Eulerian material surfaces are defined on material instances in an Eulerian section. These surfaces are available in Abaqus/Explicit for use with the general contact algorithm.
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 (Node-Based Surface Definition) 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 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.