MultiPhysicsVault/.raw/AbaqusAnalysisUserGuide1/AbaqusAnalysisUserGuide1_023.md

2.3.2 ELEMENT-BASED SURFACE DEFINITION

Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE

References

• “Surfaces: overview,” Section 2.3.1
• “Integrated output section definition,” Section 2.5.1
• “Distributed loads,” Section 34.4.3
• “Prescribed assembly loads,” Section 34.5.1
• “Mesh tie constraints,” Section 35.3.1
• “Coupling constraints,” Section 35.3.2
• “Shell-to-solid coupling,” Section 35.3.3
• “Contact interaction analysis: overview,” Section 36.1.1
• “Cavity radiation,” Section 41.1.1
• *SURFACE
• “What is a surface?,” Section 73.2.3 of the Abaqus/CAE User’s Guide

Overview

An element-based surface:

• can be defined on solid, structural, rigid, surface, gasket, or acoustic elements;
• can be deformable or rigid;
• can be defined on any combination of elements in many cases;
• can be defined on the exterior of any body; and
• can be defined on the interior of any body that is modeled with continuum, shell, membrane, surface, beam, pipe, truss, or rigid elements (e.g., to define a cross-section through a body) either by simply cutting the body with a plane or by identifying the elements and the corresponding interior facets.

For details about defining node-based surfaces, see “Node-based surface definition,” Section 2.3.3. For details about defining analytical rigid surfaces, see “Analytical rigid surface definition,” Section 2.3.4. For details about defining surfaces using Boolean combinations of existing surfaces, see “Operating on surfaces,” Section 2.3.6.

Defining element-based surfaces

You must assign a name to all element-based surfaces; this name can be used with various features to define a contact model, a surface-based load, or a surface-based constraint. In addition, you must specify the region of your model on which the surface is defined. In an input file you can define element-based surfaces on element faces, edges, or ends. In Abaqus/CAE you can define element-based surfaces on

geometric or element faces, edges, or ends. The methods for defining surfaces depend on the underlying element type and are discussed later in this section.

In an input file you need only specify an element number or element set name and all exposed element faces of these elements (or “contact edges” of beam, pipe, and truss elements) will be included in the surface. Optionally(and the only available method in Abaqus/CAE), you can specify individual faces, edges, or ends, which allows you direct control over which faces, edges, or ends are to be included in the surface.

For general contact in Abaqus/Explicit the surface perimeter edges are generated automatically from the surface facets for use in edge-to-edge contact constraints; you can specify that geometric feature edges should be included as well (see “Defining general contact interactions in Abaqus/Explicit,” Section 36.4.1, and “Assigning surface properties for general contact in Abaqus/Explicit,” Section 36.4.2, for more information).

Input File Usage: *SURFACE, NAME=surface_name, TYPE=ELEMENT (default)

An element number or element set name is specified as the first entry of each data line. Optionally, an element face, edge, or end identifier can be specified as the second entry on a data line. The face and edge identifiers used in Abaqus are discussed later in this section.

Multiple data lines can be used to define a surface. For example, SURF_1 can be specified by the following input:

* SURFACE, NAME=SURF_1, TYPE=ELEMENT
ELSET_1,
ELSET_2, S2

Abaqus/CAE Usage: Any module except Sketch, Job, and Visualization: Tools→Surface→Create: Name: surface_name

General restrictions on element-based surfaces

Elements defining a single surface must satisfy the following rules, regardless of how the surface is used in Abaqus:

• Two-dimensional, axisymmetric, and three-dimensional elements cannot be mixed in the same surface definition.
• In Abaqus/Standard deformable elements cannot be combined with rigid elements to define a single surface, but can be combined with other deformable elements that are part of a rigid body (see “Rigid body definition,” Section 2.4.1).
• The following element types cannot be mixed with other element types in the same surface definition:

– Coupled thermal-electrical-structural elements
– Coupled temperature-displacement elements
– Heat transfer elements
– Pore pressure elements

– Coupled thermal-electrical elements
– Acoustic finite or infinite elements

• The axisymmetric solid Fourier elements with nonlinear, asymmetric deformation (CAXA elements) cannot form element-based surfaces.

Surface discretization

For element-based surfaces Abaqus uses a faceted geometry defined by the finite element mesh as the surface definition. The surface in a coarse finite element model may not be a very good approximation for contact modeling if the physical surface is curved. Therefore, sufficient mesh refinement must be used to ensure that the faceted surface is a reasonable approximation of the curved physical surface. Alternatively, some curved surface geometries may be more effectively modeled with analytical rigid surfaces (see “Analytical rigid surface definition,” Section 2.3.4).

Creating surfaces on solid, continuum shell, and cohesive elements

There are three ways to define the facets of an element-based surface on solid, continuum shell, and cohesive elements:

1. by instructing Abaqus to generate the “free surface” from the exposed faces of elements,
2. by specifying the particular faces for each element, and
3. in Abaqus/Explicit by instructing Abaqus to generate an interior surface from element faces that are not exposed (i.e., not part of the “free surface” of the model).

The automatic free surface generation approach is the simplest method of defining exterior surfaces on solid elements. Specifying the element faces gives you exact control over which element faces (any combination of exterior and interior faces) form the surface. Automatic generation of an interior surface is the simplest method of defining interior surfaces on solid elements (interior surfaces can be useful for modeling surface erosion due to element failure).

It is possible to use all three approaches in the same surface definition when creating a single surface.

Generating the free surface automatically

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,” Section 35.2.2) 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 2.3.2–1 are used in linear, mesh-refinement constraints. The surfaces generated with and without multi-point constraints are shown in Figure 2.3.2–1.

flowchart

graph TD
    A["Surface SURF generated by specifying element set REFINED"] --> B["element set "REFINED""]
    B --> C["resulting surface "SURF""]
    D["without MPCs"] --> E["element set "REFINED""]
    E --> F["resulting surface "SURF""]

Figure 2.3.2–1 Effect of multi-point constraints on automatic surface generation.

Input File Usage:

*SURFACE, NAME=surface_name, TYPE=ELEMENT element number or element set,

For example, if the name of the shaded element set in Figure 2.3.2–2 is ESETA, the surface named ASURF is specified by

*SURFACE, NAME=ASURF, TYPE=ELEMENT ESETA,

Abaqus/CAE Usage: The automatic free surface generation method is not supported in Abaqus/CAE.

Special treatment of cohesive elements for automatic free surface generation

The definition of exposed faces of elements for the purpose of automatic free surface generation has the following unique aspects regarding cohesive elements:

• Faces of non-cohesive elements along an interface of shared nodes with cohesive elements are considered exposed.
• The top and bottom faces of all cohesive elements are considered exposed; side faces of cohesive elements are never considered exposed.

See “Modeling with cohesive elements,” Section 32.5.3, for examples of surfaces on or near cohesive elements.

flowchart

graph TD
    A["user-specified element set"] --> B["FEM model"]
    B --> C["perimeter"]
    C --> D["automatically generated surface"]

Figure 2.3.2–2 Automatic free surface generation.

Creating surface facets by specifying solid, continuum shell, and cohesive element faces

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

Input File Usage:

*SURFACE, NAME=surface_name, TYPE=ELEMENT element number or set, face identifier

Element face numbers are defined in Part VI, “Elements.” Table 2.3.2–1 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. When you specify the element faces to define surfaces, the specified elements cannot be a mixture of continuum and structural elements; however, each data line of the surface definition can refer to different element types.

Abaqus/CAE Usage: Any module except Sketch, Job, and Visualization: Tools→Surface→Create: Name: surface_name, pick faces in viewport

Generating an interior surface automatically

In Abaqus/Explicit you can define the facets of a surface on the interior of a solid element mesh. The faces of the specified elements that are not on the exterior (free) surface of the model will be included in the surface definition. For example, interior surfaces are used with the general contact algorithm in Abaqus/Explicit for modeling surface erosion due to element failure (see “Defining general contact interactions in Abaqus/Explicit,” Section 36.4.1).

Table 2.3.2–1 Surface definition face identifier labels for solid, continuum shell, and cohesive elements.

Elements		Face Labels
DCCAX2(D)		SPOS, SNEG
CPEG3(H)(T)	CPEG6(M)(H)(T)	S1, S2, S3
CPS3(T)	CPS6M(T)
CPE3(H)(T)	CPE6(M)(H)(T)
CAX3(H)(T)	CAX6(M)(H)(T)
CGAX3(H)	CGAX6(M)(H)(T)
AC2D3	AC2D6
ACAX3	ACAX6
DC2D3(E)	DC2D6(E)
DCAX3(E)	DCAX6(E)
CGAX4(R)(H)(T)	CGAX8(R)(H)	S1, S2, S3, S4
CPEG4(H)(I)(R)(T)	CPEG8(R)(H)(T)
CPS4(I)(R)(T)	CPS8(R)(T)
CPE4(H)(I)(R)(T)(P)	CPE8(H)(R)(T)(P)
CAX4(H)(I)(R)(T)(P)	CAX8(R)(H)(T)(P)
C3D4(H)(T)	C3D10(M)(H)(I)(T)
AC2D4(R)	AC2D8
ACAX4(R)	ACAX8
AC3D4	AC3D10
DC2D4(E)	DC2D8(E)
DCAX4(E)	DCAX8(E)
DC3D4(E)	DC3D10(E)
DCC2D4(D)	DCCAX4(D)
COH2D4	COHAX4
C3D6(H)(T)	C3D15(H)(V)	S1, S2, S3, S4, S5
AC3D6	AC3D15
CCL9(H)	CCL18(H)
DC3D6(E)	DC3D15(E)
SC6R	COH3D6
C3D8(H)(I)(R)(T)(P)	C3D20(H)(R)(T)(P)	S1, S2, S3, S4, S5, S6
C3D27(R)(H)	AC3D20
AC3D8(R)	CCL24(R)(H)
CCL12(H)	DC3D20(E)
DC3D8(E)	COH3D8
DCC3D8(D)
SC8R

The automatic generation of an interior surface is equivalent to constructing a surface consisting of all faces of the elements and then subtracting the free surfaces of those elements. Shell elements, beam elements, pipe elements, membrane elements, etc. are ignored since they do not have any interior faces by definition.

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.

Input File Usage:

*SURFACE, NAME=surface_name, TYPE=ELEMENT

element number or element set, INTERIOR

For example, if the name of the shaded element set in Figure 2.3.2–3 is ESETA, the surface named ASURFINTR (the elements in the figure have been reduced in size to differentiate faces that share the same nodes) is specified by

*SURFACE, NAME=ASURFINTR, TYPE=ELEMENT ESETA, INTERIOR

Abaqus/CAE Usage:

Any module except Sketch, Job, and Visualization: Tools→Surface→Create:

Name: surface_name, Type: Mesh; pick element faces or edges from an interior surface

You can use the selection tools to select from an interior entity of a model; see “Selecting interior surfaces,” Section 6.2.12 of the Abaqus/CAE User’s Guide.

text_image

FEM model user-specified element set ⇒ surface ASURFINTR drawn with solid lines

Figure 2.3.2–3 Automatic interior surface generation.

There are five ways to define surfaces on structural, surface, and rigid elements:

1. You can create a single-sided surface with a well-defined orientation by indicating either the top or bottom surface of each specified element.
2. You can create a double-sided surface by specifying only the elements and letting Abaqus generate the “free surface” from the exposed faces.
3. You can create an edge-based surface.
4. You can create a cross-section surface on the ends of beam, pipe, and truss elements.
5. You can create a three-dimensional curve-type surface along the length of beam, pipe, and truss elements by specifying only the elements and letting Abaqus generate the “free surface.”

It is possible to use any or all of the above approaches in the same surface definition as long as it makes sense in the use of that surface with other features in Abaqus. Table 2.3.2–2 contains a list of valid face and edge identifiers for structural, surface, and rigid elements.

Table 2.3.2–2 Surface definition face and edge identifier labels for structural, surface, and rigid elements.

Elements		Face and Edge Labels
SAX1	SAX2(T)	SPOS, SNEG
MAX1	MAX2
MGAX1	MGAX2
M3D6	M3D8(R)
M3D9(R)	MCL6
MCL9	DS4
DS8	DSAX1
DSAX2	SFMAX1
SFMAX2	SFMGAX1
SFMGAX2	SFM3D3
SFM3D4(R)	SFM3D6
SFM3D8(R)	SFMCL9
SFMCL6	RAX2
B21(H)	B22(H) (Abaqus/Standard)	SPOS, SNEG
B23(H)	PIPE22(H)
PIPE21(H)	T2D3(H)(T)
T2D2(H)(T)

Elements		Face and Edge Labels
B22 (Abaqus/Explicit)	B31(H)(OS)	END1, END2; must use node-based surfaces with the contact pair algorithm in Abaqus/Explicit.
B32(H)(OS)	B33(H)
ELBOW31(B)(C)	ELBOW32
PIPE31(H)	PIPE32(H)
T3D2(H)(T)	T3D3(H)(T)
STRI3	STRI65	SPOS, SNEG, E1, E2, E3
S3(R)(S)	R3D3
M3D3
ACIN2D2	ACIN2D3	SPOS
ACINAX2	ACINAX3	E1, E2
S4(R)(S)(W)(5)	S8R5(T)	SPOS, SNEG, E1, E2, E3, E4
S9R5	R3D4
M3D4(R)
ACIN3D3	ACIN3D6	SPOS
		E1, E2, E3
ACIN3D4	ACIN3D8	SPOS
		E1, E2, E3, E4

Defining single-sided surfaces

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 Part VI, “Elements.”

You must ensure that all of the specified elements have their normals oriented consistently. If they are oriented as shown in Figure 2.3.2–4, 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. 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.

Input File Usage:

Use the following option to define a surface on the positive face of a structural, surface, or rigid element:

*SURFACE, NAME=surface_name, TYPE=ELEMENT element number or element set, SPOS

Use the following option to define a surface on the negative face of a structural, surface, or rigid element:

text_image

element set SHELL element normals

Figure 2.3.2–4 Inconsistent orientation of structural element normals can result in an invalid surface.

*SURFACE, NAME=surface_name, TYPE=ELEMENT element number or element set, SNEG

For example, single-sided surfaces on the positive faces of the elements in element set SHELL can be defined using input similar to

*SURFACE, NAME=BSURF, TYPE=ELEMENT SHELL, SPOS

Abaqus/CAE Usage: Any module except Sketch, Job, and Visualization: Tools→Surface→Create: Name: surface_name, pick face in viewport, click mouse button 2, and specify the side of the selected face

Defining double-sided surfaces

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” in “Defining contact pairs in Abaqus/Explicit,” Section 36.5.1).