Element-Based Surface Definition

You can define the facets of a surface by specifying a series of elements. The faces of these elements that are on the exterior (free) surface of the model are included in the surface definition.

When the free surface generation method is used to define surfaces, the specified elements can be a mixture of continuum and structural elements.

Multi-point constraints (General Multi-Point Constraints) involving nodes on exposed surfaces are not taken into account during free surface generation, which can result in faces that are not on the exterior of a body being included in surface definitions. For example, the nodes of the elements in element set REFINED shown in Figure 1 are used in linear, mesh-refinement constraints. The surfaces generated with and without multi-point constraints are shown in Figure 1.

Effect of multi-point constraints on automatic surface generation.

You can define the facets of a surface by identifying the element faces that should be included in the surface definition.

Element face numbers are defined in About the Element Library. Table 1 contains a list of valid face identifiers for all solid, continuum shell, and cohesive elements. The face identifier can refer to individual elements or to entire element sets.

Abaqus/Explicit provides two approaches to define eroding surfaces for a solid element mesh for use in general contact (see Modeling Surface Erosion). The recommended approach dynamically evolves the list of surface faces to correspond to currently exposed faces of elements that have not failed. The other approach statically creates all of the possible interior faces and tracks which of these faces are active. These methods give approximately the same results, but the dynamically evolving approach often uses much less memory and tends to be faster.

Elements that do not have any interior faces by definition (such as shell elements, beam elements, pipe elements, and membrane elements) are ignored.

Multi-point constraints are not taken into account when generating interior surfaces. This can result in faces that are on the interior of a body being excluded from the surface definition.

You can define a single-sided surface on the positive or negative face of structural, surface, or rigid elements. The positive face is defined as the one in the direction of the positive element normal, and the negative face is defined as the one in the direction opposite to the element normal. The definition of the element normal for all elements is given in About the Element Library.

You must ensure that all of the specified elements have their normals oriented consistently. If they are oriented as shown in Figure 2, the surface normals will reverse direction as the surface is traversed and improper results may occur when the surface is used with features requiring an orientation such as distributed surface loads.

Inconsistent orientation of structural element normals can result in an invalid surface.

Further, an error message will be issued and the analysis will terminate if this condition is detected for surfaces used with mesh tie constraints in Abaqus/Standard or with contact pairs. To correct the surface orientations in this figure, two separate element sets with different face identifiers should be used.

You can create double-sided surface facets on three-dimensional shell, membrane, surface, and rigid elements using the automatic surface facet generation approach (i.e., specifying only the element numbers or sets). Some applications that refer to surfaces do not allow the use of double-sided surfaces: examples include contact pairs in Abaqus/Standard and features requiring an oriented surface such as distributed surface loads. When double-sided surfaces can be used, they are often preferred to single-sided surfaces. In some applications, such as when defining the contact domain for general contact, it does not matter whether single- or double-sided surfaces are used.

When double-sided surfaces are used with contact pairs in Abaqus/Explicit, the normals of all the underlying elements do not need to have a consistent positive orientation: Abaqus/Explicit will define the contact surface such that its facets have consistent normals, even if the underlying elements do not have consistent normals. The facet normals will be the same as the element normals if the element normals are all consistent; otherwise, an arbitrary positive orientation is chosen for the surface. The positive orientation is significant only with respect to the sign of the contact pressure output variable for the contact pair algorithm, CPRESS (see Output).

Although contact is enforced unconditionally on both sides of a surface when self-contact is used with contact pairs, contact is enforced on both sides of a surface used in two-body contact only when that surface is double-sided (if allowed). The use of single-sided surfaces with contact pairs is sometimes desirable: the resolution of large initial overclosures in contact pairs is more robust with single-sided surfaces than with double-sided surfaces (see Contact Initialization for Contact Pairs in Abaqus/Explicit). However, single-sided contact is generally more limiting than double-sided contact; it may cause an analysis to fail due to excessive element distortion or not enforce the contact conditions realistically if a secondary node unexpectedly moves behind a main surface. This condition can occur, for example, when large deformations or rigid-body motions are present or due to complex tool shapes in a forming analysis.

You can define an edge-based surface on three-dimensional shell, membrane, surface, or rigid elements by specifying the individual edges. Alternatively, you can specify that all the edges of the elements that are on the exterior (free) surface of the model are used to form the surface; this method cannot be used to define edge-based surfaces that are in the interior of the model. It is possible to use both methods in the same surface definition when creating a single surface.

To define a surface over the cross-section of beam, pipe, or truss elements, you must specify the end on which the surface is defined. Surfaces created on the ends of these elements can be used only for integrated output request (see Integrated Output) and integrated output section (see Integrated Output Section Definition) definitions.

You cannot specify the faces to define a surface along the length of three-dimensional beams, pipes, or trusses because their element connectivity cannot define a unique element or surface normal. Instead, you must specify that Abaqus should generate a surface for these elements. Therefore, the use of surfaces along the length of these elements is restricted.

In Abaqus/Standard element-based surfaces created along the length of three-dimensional beam, pipe, or truss elements can be used with the general contact algorithm or tie constraints. In a contact pair simulation, they can be used only as secondary surfaces. There are several advantages to using an element-based surface rather than a node-based surface when modeling contact in Abaqus/Standard with three-dimensional beams, pipes, or trusses:

1. The default local tangent directions are parallel and orthogonal to the element axis.

2. Abaqus/Standard calculates the contact results as contact forces per unit length rather than just contact forces.

3. It can be easier to define an element-based surface than a node-based surface.

In Abaqus/Standard a surface definition is not allowed for cases where three or more three-dimensional beams, pipes, or trusses are joined at a common node because of the lack of uniquely defined element tangents.

In Abaqus/Explicit element-based surfaces created along the length of three-dimensional beam, pipe, or truss elements can be used only with the general contact algorithm or tie constraints. To define contact for these elements using the contact pair algorithm, the nodes forming the beam, pipe, or truss elements can be included in a node-based surface definition (Node-Based Surface Definition) and a contact pair can be defined for this node-based surface and a non-node-based surface.

Surfaces along the length of three-dimensional beam, pipe, or truss elements cannot be used to prescribe a distributed surface load since the loading direction is not unique.

Surfaces created along the length of two-dimensional beam, pipe, and truss elements can be used as main surfaces in a contact pair simulation because the underlying elements have unique element normals that lie in the plane of the model. These surfaces can also be used to prescribe distributed surface loads.

Some applications that refer to surfaces will account for underlying element thicknesses and any offset of the midsurface relative to the reference surface for surfaces based on shell, membrane, or rigid elements. For example, all of the contact algorithms available in Abaqus/Explicit can account for these effects. Of the contact algorithms available in Abaqus/Standard, only the surface-to-surface small-sliding contact formulation can account for these effects. See the following sections for additional details on applications that can account for surface thickness and offset:

• Mesh Tie Constraints

• Contact Formulations in Abaqus/Standard

• Assigning Surface Properties for General Contact in Abaqus/Explicit

• Assigning Surface Properties for Contact Pairs in Abaqus/Explicit

There are several advantages to using an element-based surface rather than a node-based surface when modeling contact in Abaqus/Standard with three-dimensional gasket line elements:

1. The local tangent directions are parallel and orthogonal to the gasket line element, which is useful for output purposes and for anisotropic friction definition.

2. Abaqus/Standard calculates the contact results as contact forces per unit length rather than just contact forces.

Surfaces created on three-dimensional gasket line elements can be used only as secondary surfaces because Abaqus/Standard cannot form unique normals for these surfaces.

The effect of surface trimming is best explained by means of an example. Figure 3 illustrates the effect of trimming for two different surfaces defined on the same simple two-dimensional mesh.

Case I: Faces A and B are removed when trimming is done since one node of each of the faces is an end node and the other is a corner node. Case II: Faces A and B are not removed when trimming is done since one node of each of the faces is an end node but the other is not a corner node.

In Case I the surface definition consists of a single layer of elements on the perimeter of the model. Using automatic surface facet generation, the resulting default surface (curve) includes the vertical element faces A and B since these faces lie on the perimeter of the model. Trimming the default surface created in Case I eliminates faces A and B since their presence results in the two spurious corners near the perimeter of the curve.

Abaqus uses a special criterion in deciding to remove faces A and B from the original open curve. A face is removed if one of its end nodes is an endpoint and either of the following is true: another face node is a node on an element corner belonging to the curve or the face normal differs by more than 30° from the normal of an adjacent face also belonging to the curve. To be a node on an element corner belonging to the curve means to be a node on two different faces of the same element, both of which are part of the curve. The face removal criterion is applied recursively to the curve definition until all corners on or near the perimeter of the curve have been removed. This procedure is generalized for three-dimensional surface definitions.

In Case II in Figure 3 trimming would not result in the elimination of faces A and B because neither of the endpoints of these two faces meets the criterion described above.

Trimming of surfaces used for application of distributed loads is usually desired since loads are normally applied to specific sides of a body. Any surface that is used for application of a distributed load will, by default, be trimmed.

In Abaqus/Standard trimming the secondary surface in contact or interaction simulations results in more accurate estimates of the contact pressures, heat fluxes, and electrical current densities along the perimeter of the surface. Any surface that is used as a secondary surface in a contact or interaction simulation will, by default, be trimmed. If the secondary surface is left untrimmed, the nodes at the corners of the surface will be assigned additional contact area from the element faces around the corners that may never be involved in the interaction between the surfaces. This additional contact area introduces errors into the estimates of the contact output variables at those nodes. Main surfaces in small-sliding simulations will, by default, be trimmed; Abaqus/Standard will normally form a better approximate surface. However, main surfaces in finite-sliding contact simulations will, by default, be left untrimmed, and they should extend far enough away from all expected regions of contact. This practice protects against the possibility of the secondary surface nodes sliding off the main surface (see Common Difficulties Associated with Contact Modeling in Abaqus/Standard).