김경종
17 KiB
Special considerations when defining orientations on contact surfaces in Abaqus/Standard
When a user-defined orientation is used to define the local tangent directions on a surface of a three-dimensional contact pair in Abaqus/Standard (see “Contact formulations in Abaqus/Standard,” Section 38.1.1), you cannot define points a and b by giving local node numbers (see Figure 2.2.5–1).
For geometrically nonlinear analysis the local tangent directions of a contact pair rotate with the surface on which the directions were defined initially. These rotated local tangent directions are further rotated to ensure that the normal vector, computed using the cross product of the rotated local tangent directions, corresponds to the normal vector on the master surface when the slave node comes into contact.
Arbitrary local tangent directions can be defined for a “line”-type slave surface defined on threedimensional beam, truss, or pipe elements. When this surface comes into contact with the master surface during a large-displacement analysis, the local tangent directions are projected onto the master surface.
Use with laminated shells
There are two ways in which a user-defined orientation can be used in the section definition of a laminated shell. In each case the name referenced in the shell section definition is the name of the user-defined orientation.
The first is to associate the user-defined orientation with the entire composite shell section definition. Then each layer’s orientation angle can be given relative to this section orientation (or the default shell coordinate directions if no section orientation is used). The angle is given as an additional rotation about the shell normal after the orientation directions have been projected onto the shell surface. Section forces (available only from Abaqus/Standard) are given in the local system specified for the section.
The second is to specify the name of each layer’s orientation separately; this method allows different orientation definitions to be referenced for the different layers. Section forces and strains are still reported in the local orientation defined for the entire section (or the default shell coordinate directions if no section orientation is used). The individual layer orientations are used for material calculations and for output of stress and strain.
See “Using a shell section integrated during the analysis to define the section behavior,” Section 29.6.5, and “Using a general shell section to define the section behavior,” Section 29.6.6, for more information.
Use with laminated three-dimensional solid elements
When a user-defined orientation is used with composite solid elements (available only in Abaqus/Standard), one of the local directions must be identified as the axis for additional rotation. There are two ways in which this orientation can be used with a composite solid section definition to specify the material orientation for individual layers. In each case the name referenced in the solid section definition is the name of the user-defined orientation.
The first is to associate the user-defined orientation with the entire composite solid section definition. Then each layer’s orientation angle can be given relative to this section orientation. The angle is given as an additional rotation about the local direction defined as the axis for additional rotation.
The second is to specify the name of each layer’s orientation separately; this method allows different orientation definitions to be referenced for the different layers. (In this case any user-defined orientation associated with the entire solid section will be ignored.)
See “Defining the element’s section properties” in “Solid (continuum) elements,” Section 28.1.1, for more information.
Use with pipe-soil interaction elements
An arbitrary user-defined orientation can be defined for pipe-soil interaction elements (available only in Abaqus/Standard). In a large-displacement analysis the local orientation system rotates with the rigid body motion of the underlying pipeline. In a small-displacement analysis the local system is defined by the initial geometry of the PSI element and remains fixed in space during the analysis.
Use with beam, frame, and truss elements
See “Beam element cross-section orientation,” Section 29.3.4, for information on defining local material directions for beams, frames, or trusses.
Use with the fabric material model
The fill and the warp yarn directions in the fabric plane are allowed to rotate with respect to each other under shear deformations (“Fabric material behavior,” Section 23.4.1). The current yarn directions are tracked with respect to the orthogonal coordinate system that also rotates with the material.
Use with the jointed material model
When a user-defined orientation is used to define a joint system orientation for the jointed material model available in Abaqus/Standard (“Jointed material model,” Section 23.5.1), only the local coordinate system need be defined. It is assumed that the first direction is the direction normal to the plane of the joint and the other directions are in the plane of the joint. An additional axis of rotation cannot be used.
Use with rotary inertia and connector elements
A user-defined orientation must be used to define the local directions for certain connection types used to define connector elements (see “Connection-type library,” Section 31.1.5).
A user-defined orientation can be used with SPRING1, SPRING2, DASHPOT1, DASHPOT2, JOINTC, JOINT2D, JOINT3D, and ROTARYI elements to provide a local system for defining the direction of action of such elements. Points a, b, and c (see Figure 2.2.5–1) cannot be defined by giving local node numbers when the orientation is used for these elements. If you do not specify an axis for additional rotation, the local 1-direction with no additional rotation will be chosen as the default.
Use with the kinematic coupling constraint
User-defined orientations can be used in Abaqus/Standard to define the local coordinate systems in which constraint directions are specified for a kinematic coupling constraint (see “Kinematic coupling
constraints,” Section 35.2.3). In this case you cannot define points a, b, and c by giving local node numbers (see Figure 2.2.5–1).
Use with surface-based coupling constraints
User-defined orientations can be used to define the local coordinate systems in which surface-based coupling constraint directions are specified (see “Coupling constraints,” Section 35.3.2). In this case you cannot define points a, b, and c by giving local node numbers (see Figure 2.2.5–1).
Use with inertia relief
A user-defined orientation can be used in Abaqus/Standard to define a local system of directions along which the inertia relief loads are computed (see “Inertia relief,” Section 11.1.1). In this case you cannot define points a, b, and c by giving local node numbers (see Figure 2.2.5–1).
Use with distributed general traction, shear traction, and general edge loads
User-defined orientations can be used in Abaqus to define the local coordinate systems in which the loading directions for distributed general tractions, shear tractions, and general edge loads are specified. See “Distributed loads,” Section 34.4.3.
Orientations defined with distributions
Spatially varying local coordinate systems (for material definitions, material calculations, and output) defined with a distribution can be applied only to solid continuum, membrane (in Abaqus/Standard), and shell elements. See “Solid (continuum) elements,” Section 28.1.1; “Membrane elements,” Section 29.1.1; “Using a shell section integrated during the analysis to define the section behavior,” Section 29.6.5; and “Using a general shell section to define the section behavior,” Section 29.6.6.
Output
When a user-defined orientation is used in an element section definition, the stress, the strain, and the element section force components are output in the local system.
For a fabric material the output of the regular material point tensors such as stress and strain are given in an orthogonal coordinate system even when the local yarn directions are non-orthogonal. However, the nominal fabric stress SFABRIC and the nominal fabric strain EFABRIC are also available for output (see “Fabric material behavior,” Section 23.4.1).
This use of a local system is indicated by a footnote in the printed output tables from Abaqus/Standard. An orientation used with the jointed material model does not affect the output.
When a user-defined orientation is used in Abaqus/Standard with kinematic or distributing coupling constraints, the local system is indicated in the analysis input file processor output tables.
Local coordinate systems are written automatically to the output database with the exception of systems defined by specifying points a and b relative to local or global node numbers or systems defined through a user subroutine. Any additional rotations specified are ignored.
ORIENTATIONS
Material directions are written automatically to the output database. They can also be written to the Abaqus/Standard results file (with at least one output variable specified; see “Output of local directions to the results file” in “Output to the data and results files,” Section 4.1.2). The material directions can be visualized in Abaqus/CAE by selecting Plot→Material Orientations in the Visualization module.
2.3 Surface definition
• “Surfaces: overview,” Section 2.3.1
• “Element-based surface definition,” Section 2.3.2
• “Node-based surface definition,” Section 2.3.3
• “Analytical rigid surface definition,” Section 2.3.4
• “Eulerian surface definition,” Section 2.3.5
• “Operating on surfaces,” Section 2.3.6
2.3.1 SURFACES: OVERVIEW
Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE
References
• “Element-based surface definition,” Section 2.3.2
• “Node-based surface definition,” Section 2.3.3
• “Analytical rigid surface definition,” Section 2.3.4
• “Eulerian surface definition,” Section 2.3.5
• “Operating on surfaces,” Section 2.3.6
• “Integrated output section definition,” Section 2.5.1
• “Acoustic, shock, and coupled acoustic-structural analysis,” Section 6.10.1
• “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
• “Defining tied contact in Abaqus/Standard,” Section 36.3.7
• “Cavity radiation,” Section 41.1.1
Overview
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, an Eulerian material instance, or element faces, edges, or ends; and
• can be deformable, rigid, or partially deformable and partially rigid.
This section describes the general rules that apply when creating surfaces in Abaqus.
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 userdefined 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,” 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 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.
Internal surfaces created by Abaqus/CAE
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 78, “Using display groups to display subsets of your model,” of the Abaqus/CAE User’s Guide).
Input File Usage: *SURFACE, NAME=surface_name, INTERNAL
Restrictions on surfaces
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:
• “Integrated output section definition,” Section 2.5.1
• “Distributed loads,” Section 34.4.3
• “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
• “Defining contact pairs in Abaqus/Standard,” Section 36.3.1
• “Defining general contact interactions in Abaqus/Explicit,” Section 36.4.1
• “Defining contact pairs in Abaqus/Explicit,” Section 36.5.1
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 2.10.1.