김경종
22 KiB
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 “Adjusting initial surface positions and specifying initial clearances for contact pairs in Abaqus/Explicit,” Section 36.5.4). 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 slave node unexpectedly moves behind a master 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.
Input File Usage: Use the following option to define a double-sided surface on three-dimensional shell, membrane, surface, or rigid elements in Abaqus/Explicit:
*SURFACE, NAME=surface_name, TYPE=ELEMENT element number or element set,
For example, double-sided surfaces on the elements in element set SHELL can be defined using input similar to
*SURFACE, NAME=BSURF, TYPE=ELEMENT SHELL,
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 choose Both sides
Defining edge-based surfaces
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.
Input File Usage: Use the following option to specify the individual edges that form the surface:
*SURFACE, NAME=surface_name, TYPE=ELEMENT element number or element set, edge identifier
The individual edge identifiers used in Abaqus are listed in Table 2.3.2–2.
Use the following option to specify that all the edges of the elements that are on the exterior (free) surface of the model are used to form the surface:
*SURFACE, NAME=surface_name, TYPE=ELEMENT element number or element set, EDGE
For example, if the shaded element set in Figure 2.3.2–2 is composed of threedimensional shell elements and is named ESETA, the surface named ESURF could be specified by the following input:
*SURFACE, NAME=ESURF, TYPE=ELEMENT ESETA, EDGE
Abaqus/CAE Usage: Any module except Sketch, Job, and Visualization: Tools→Surface→Create: Name: surface_name, pick edges in viewport
In Abaqus/CAE 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 by directly picking all the free edges in the viewport.
Defining a surface over the cross-section at the ends of beam, pipe, and truss elements
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” in “Output to the output database,” Section 4.1.3) and integrated output section (see “Integrated output section definition,” Section 2.5.1) definitions.
Input File Usage: Use the following option to define a surface over the cross-section of a beam, pipe, or truss element:
*SURFACE, NAME=surface_name, TYPE=ELEMENT element number or element set, END1 or END2
Abaqus/CAE Usage: Any module except Sketch, Job, and Visualization: Tools→Surface→Create: Name: surface_name, pick three-dimensional wire region in viewport, click mouse button 2, and choose End (Magenta) or End (Yellow)
Defining a surface along the length of three-dimensional beam, pipe, and truss elements
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 in tie constraints but can be used only as slave surfaces in contact interactions. However, 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:
- The default local tangent directions are parallel and orthogonal to the element axis.
- Abaqus/Standard calculates the contact results as contact forces per unit length rather than just contact forces.
- 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,” Section 2.3.3) 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.
Input File Usage: Use the following option to define a surface along the length of a three-dimensional beam, pipe, or truss element:
*SURFACE, NAME=surface_name, TYPE=ELEMENT element number or element set,
Abaqus/CAE Usage: Any module except Sketch, Job, and Visualization: Tools→Surface→Create:
Name: surface_name, pick three-dimensional wire region in viewport, click mouse button 2, and choose Circumferential
Surfaces along the length of two-dimensional beam, pipe, and truss elements
Surfaces created along the length of two-dimensional beam, pipe, and truss elements can be used as master 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.
Shell, membrane, or rigid element thickness and shell offset
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,” Section 35.3.1
• “Contact formulations in Abaqus/Standard,” Section 38.1.1
• “Assigning surface properties for general contact in Abaqus/Explicit,” Section 36.4.2
• “Assigning surface properties for contact pairs in Abaqus/Explicit,” Section 36.5.2
Creating surfaces on gasket elements
When surfaces are defined on gasket elements, automatic surface facet generation cannot be used because only the top and bottom element faces can be used to create surfaces (see “Gasket elements: overview,”
Section 32.6.1). Abaqus/Standard cannot create surfaces on gasket link elements since the top and bottom surfaces are each reduced to a single node. For other gasket elements you must specify the top and bottom surfaces directly. The positive face of the element is in the thickness direction of the element. The definition of the thickness direction of all gasket elements is given in “Defining the gasket element’s initial geometry,” Section 32.6.4. The negative face is defined as the face in the direction opposite to the thickness direction of the element.
| Input File Usage: | Use the following option to define a surface on the positive face of a gasket element:*SURFACE, NAME=surface_name, TYPE=ELEMENTelement number or element set, SPOSUse the following option to define a surface on the negative face of a gasket element:*SURFACE, NAME=surface_name, TYPE=ELEMENTelement number or element set, SNEGFor example, single-sided surfaces on the positive faces of the elements in element set GASKET can be defined using input similar to*SURFACE, NAME=BSURF, TYPE=ELEMENTGASKET, SPOS |
| Abaqus/CAE Usage: | Any module except Sketch, Job, and Visualization: Tools→Surface→Create: Name: surface_name, pick top or bottom faces in viewport |
Surfaces on three-dimensional gasket line elements
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:
- The local tangent directions are parallel and orthogonal to the gasket line element, which is useful for output purposes and for anisotropic friction definition.
- 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 slave surfaces because Abaqus/Standard cannot form unique normals for these surfaces.
Creating interior cross-section surfaces
To study the “force-flow” through various paths in a model, you must create interior surfaces that cut through one or more components (similar to a cross-section) so that you can request integrated output of the total force transmitted across these surfaces (see “Requesting integrated output for “force-flow” studies” in “Output to the output database,” Section 4.1.3). Abaqus provides a simple method to create such an interior surface over the element facets, edges, or ends by cutting through a region of the model with a plane. The region can be identified using one or more element sets. If no element sets are specified, the region consists of the whole model. The cutting plane is defined by specifying the coordinates of a
point on the plane and a vector normal to the plane. Alternatively, the cutting plane can be defined by specifying the global node numbers of point a on the plane and point b that lies off the cutting plane with the normal determined as the vector from point a to point b. Abaqus then automatically forms a surface close to the specified cutting plane by selecting the element facets, edges, or ends of the continuum solid, shell, membrane, surface, beam, pipe, truss, or rigid elements in the selected region. The surface generated in this manner is an approximation for the cutting plane.
Multi-point mesh constraints are ignored while generating the interior surface based on the cutting plane; therefore, the result may be a surface that is not continuous if these constraints stitch disjointed meshes together in a region that is cut by the cutting plane. When the cutting plane intersects a beam, pipe, or truss element, the entire element is shown in the Visualization module of Abaqus/CAE as being part of the surface. However, if this surface is used for integrated output, only the element nodal forces from the element end that lies on the positive side as defined by the normal to the cutting plane are included in the integrated output. Point mass and rotary elements, connector elements, spot welds, and spring elements will not be part of the generated surface even if they are cut by the cutting plane.
Input File Usage: Use the following option to define the cutting surface by specifying coordinates of a point on the plane and a vector normal to the plane:
*SURFACE, NAME=surface_name, TYPE=CUTTING SURFACE, DEFINITION=COORDINATES
Use the following option to define the cutting surface by specifying global node numbers of points a and b:
*SURFACE, NAME=surface_name, TYPE=CUTTING SURFACE, DEFINITION=NODES
Abaqus/CAE Usage: Interior cross-section surfaces are not supported in Abaqus/CAE.
Whole-model free surface in an Abaqus/Explicit input file
In an Abaqus/Explicit input file you can create a surface containing the exposed faces of all elements (and “contact edges” of beam, pipe, and truss elements) in the model except cohesive elements by specifying a blank element set name and a blank face identifier. This “free” surface of the model can be used as the base surface for the cropping and combining operations; without modifications this surface is similar to the default all-inclusive surface commonly used in general contact (see “Defining general contact interactions in Abaqus/Explicit,” Section 36.4.1).
Input File Usage: *SURFACE, NAME=surface_name, TYPE=ELEMENT
Abaqus/CAE Usage: The whole-model automatic free surface generation method is not supported in Abaqus/CAE.
Trimming the perimeter of an open surface
An “open” surface is one that has ends in two dimensions or an outside edge in three dimensions. The ends of a two-dimensional surface and the edge of a three-dimensional surface are called the surface’s “perimeter.” Since Abaqus allows a surface to be defined as only a part of the surface of a body, it may
have a perimeter even though it is defined on a closed body. Abaqus automatically performs surface “trimming” on solid element meshes. You can change the default setting when a surface is created, providing some basic control over the extent of surfaces.
Surface trimming:
• is a recursive procedure that removes undesirable convex corners near the perimeter of an open surface (see the example below for details);
• has no effect on closed surfaces (ones with no ends or edges);
• is performed automatically, unless the surface is used as a master surface in a finite-sliding simulation in Abaqus/Standard or the surface is used with the contact pair algorithm in Abaqus/Explicit;
• can be used only for external surfaces on solid element meshes (either specified surfaces or automatically generated free surfaces); and
• has no effect on surfaces used with the contact pair algorithm in Abaqus/Explicit.
Input File Usage: Use the following option to suppress automatic surface trimming: *SURFACE, TYPE=ELEMENT, NAME=surface_name, TRIM=NO
Abaqus/CAE Usage: Automatic surface trimming cannot be suppressed in Abaqus/CAE.
The effect of surface trimming
The effect of surface trimming is best explained by means of an example. Figure 2.3.2–5 illustrates the effect of trimming for two different surfaces defined on the same simple two-dimensional mesh.
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 2.3.2–5 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.
Why Abaqus will, by default, trim most surfaces
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.
Figure 2.3.2–5 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 Abaqus/Standard trimming the slave 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 slave surface in a contact or interaction simulation will, by default, be trimmed. If the slave 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. Master surfaces in small-sliding simulations will, by default, be trimmed; Abaqus/Standard will normally form a better approximate surface. However, master 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 slave surface nodes sliding off the master surface (see “Common difficulties associated with contact modeling in Abaqus/Standard,” Section 39.1.2).
2.3.3 NODE-BASED SURFACE DEFINITION
Products: Abaqus/Standard Abaqus/Explicit
References
• “Surfaces: overview,” Section 2.3.1
• “Mesh tie constraints,” Section 35.3.1
• “Contact interaction analysis: overview,” Section 36.1.1
• *SURFACE
Overview
A node-based “surface”:
• can be used only as a “slave surface” in contact calculations;
• can be used as a “slave” or “master surface” in a surface-based tie constraint;
• is convenient in three-dimensional cases where Abaqus cannot construct a unique physical surface on the elements, such as a pipe modeled with pipe elements contacting the ocean floor or cables modeled with trusses contacting the ground after they break;
• should be used with caution or not at all if accurate contact stresses are needed or if heat will be exchanged between the two surfaces;
• can be assigned a nonzero thickness for use with the general contact algorithm in Abaqus/Explicit;
• should not be used to model a shell or membrane surface if the thickness and midsurface offset need to be considered in the problem;
• must either contain nodes that are all part of the same rigid body or not contain any nodes that are part of a rigid body if the node-based surface is to be used in a penalty contact pair in Abaqus/Explicit;
• in Abaqus/Standard does not provide heat conduction between surfaces in fully coupled temperature-displacement analysis or pore fluid flow between surfaces in coupled pore pressure–displacement analysis;
• in Abaqus/Standard does not provide heat conduction and electrical conduction between surfaces in a fully coupled thermal-electrical-structural analysis; and
• does not include circumferential friction when used with axisymmetric elements with twist (CGAX, MGAX elements).
Alternatives to node-based surfaces are element-based surfaces (see “Element-based surface definition,” Section 2.3.2) and, in the case of rigid surfaces, analytical rigid surfaces (see “Analytical rigid surface definition,” Section 2.3.4). See “Operating on surfaces,” Section 2.3.6, for information on defining surfaces using Boolean combinations of existing surfaces.
Creating a node-based surface
You create a node-based surface by specifying the nodes or node sets that form the surface. You must assign a name to the node-based surface; this name will be used when defining contact interactions that involve the surface.
An optional associated area can be defined for each node. If no area is defined for a node and the surface is defined in a contact pair, the area specified as part of the contact property definition is used. If no area is specified as part of the contact property definition, a unit area is used.
In Abaqus/Explicit the area used in contact pair calculations for a node in a node-based surface is always 1.0, regardless of the user-specified value. Therefore, the contact pressure output variable in Abaqus/CAE should be interpreted as the contact force when a node-based surface is used for contact pairs in Abaqus/Explicit.
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. Additional rules are given in “Defining an assembly,” Section 2.10.1.
When the nodes of shell and membrane elements are used in a node-based surface, the thickness and midsurface offset of the shell or membrane at each node are not considered. However, a nonzero thickness can be assigned to node-based surfaces when used with the general contact algorithm in Abaqus/Explicit (see “Assigning surface properties for general contact in Abaqus/Explicit,” Section 36.4.2, for more information).
Input File Usage: *SURFACE, NAME=name, TYPE=NODE
node number or node set, area