Products: ABAQUS/Standard ABAQUS/Explicit ABAQUS/CAE
A user-defined orientation is used to define a local coordinate system for:
definition of material properties—for example, anisotropic materials or jointed materials (a local coordinate system must be defined if anisotropic material properties are defined for solid elements);
definition of rebars in shell, membrane, and surface elements;
definition of rotary inertia and connector elements;
definition of coupling constraints;
definition of loading directions for distributed general tractions, shear tractions, and general edge loads;
definition of slip directions for contact in ABAQUS/Standard;
material calculations at integration points;
output of components of stress, strain, and element section force; and
definition of a local system of rigid body motion directions for inertia relief in ABAQUS/Standard.
at points where the smeared crack concrete material behavior (“Concrete smeared cracking,” Section 18.5.1) is also used in ABAQUS/Standard;
to specify a local coordinate system for defining nodal coordinates—see “Specifying a local coordinate system in which to define nodes” in “Node definition,” Section 2.1.1, or “Specifying a local coordinate system for the nodal coordinates” in “Node definition,” Section 2.1.1, instead; or
to specify a local coordinate system for applying loads and boundary conditions—see “Transformed coordinate systems,” Section 2.1.5, instead.
You must assign a name to each orientation definition. This name is used by various features to refer to the orientation definition.
| Input File Usage: | *ORIENTATION, NAME=name |
| ABAQUS/CAE Usage: | Any module: Tools |
In a model defined in terms of an assembly of part instances, you can define a local orientation at the part, part instance, or assembly level. An orientation defined at the part or part instance level is rotated according to the positioning data given for each instance of that part (or for the part instance). See “Defining an assembly,” Section 2.9.1.
A two-stage process is used to define the local system directly.
You define the local coordinate system at the particular location at which it is required. You can select a rectangular, cylindrical, or spherical coordinate system. The coordinate system is defined in terms of points a, b, and c, as shown in Figure 2.2.5–1. You can select the method for defining points a, b, and c, as described below.
Optionally, you can specify an additional rotation by identifying one of these local directions (
, 
, or 
) as a rotation axis and giving a rotation, in degrees, about that axis. The local system is then rotated through this angle about the specified axis. This method of defining a local system is required for contact surfaces in ABAQUS/Standard, shells, membranes, gasket elements, and when the orientation is associated with a composite solid section. The additional rotation is illustrated in Figure 2.2.5–2.
Rectangular, cylindrical, and spherical coordinate systems are available.
A rectangular Cartesian coordinate system is shown in Figure 2.2.5–1(a). The rectangular coordinate system is the default. Alternatively in ABAQUS/Standard, you can define a rectangular Cartesian coordinate system as shown in Figure 2.2.5–1(d).
| Input File Usage: | *ORIENTATION, NAME=name, SYSTEM=RECTANGULAR |
*ORIENTATION, NAME=name, SYSTEM=Z RECTANGULAR |
| ABAQUS/CAE Usage: | Any module: Tools |
A cylindrical coordinate system is shown in Figure 2.2.5–1(b). The local axes are =radial, =tangential, =axial.
| Input File Usage: | *ORIENTATION, NAME=name, SYSTEM=CYLINDRICAL |
| ABAQUS/CAE Usage: | Any module: Tools |
A spherical coordinate system is shown in Figure 2.2.5–1(c). The local axes are =radial, =circumferential, =meridional.
| Input File Usage: | *ORIENTATION, NAME=name, SYSTEM=SPHERICAL |
| ABAQUS/CAE Usage: | Any module: Tools |
You can define a coordinate system by specifying the locations of points a, b, and c directly; by specifying the locations of points a, b, and c relative to global node numbers; by specifying the locations of points a, b, and c relative to local node numbers; by specifying an offset from another coordinate system; or by specifying two lines in the coordinate system.
You can specify the coordinates of points a, b, and c directly. These coordinates should be appropriate to the system chosen. This method is the default.
You can define a rectangular Cartesian coordinate system 
by specifying three points (a, b, and c) that lie on the - plane, as shown in Figure 2.2.5–1(a). Point c is the origin of the system, point a must lie on the -axis, and point b must lie on the - plane. Although not necessary, it is intuitive to select point b such that it is on or near the local -axis.
Alternatively in ABAQUS/Standard you can define a rectangular Cartesian coordinate system by specifying three points (a, b, and c) that lie on the - plane, as shown in Figure 2.2.5–1(d). Point c is the origin of the system, point a must lie on the -axis, and point b must lie on the - plane. Although not necessary, it is intuitive to select point b such that it is on or near the local -axis.
For rectangular coordinate systems the default location of the origin (point c) is the global origin.
You define a cylindrical coordinate system by giving the two points, a and b, on the polar axis of the cylindrical system, as shown in Figure 2.2.5–1(b).
You define a spherical coordinate system by giving the center of the sphere, a, and point b on the polar axis, as shown in Figure 2.2.5–1(c).
| Input File Usage: | *ORIENTATION, NAME=name, DEFINITION=COORDINATES |
| ABAQUS/CAE Usage: | Any module: Tools |
You can locate points a, b, and c at nodes by specifying three global node numbers. For a rectangular coordinate system the default location of the origin (point c) is the global origin.
| Input File Usage: | *ORIENTATION, NAME=name, DEFINITION=NODES |
| ABAQUS/CAE Usage: | You cannot define a coordinate system by giving global node numbers in ABAQUS/CAE. |
You can locate points a, b, and c by specifying the local node numbers of an element. Local node numbers refer to the order in which nodes are specified in the element connectivity. For example, local node number 2 corresponds to the second node specified for the element definition. This definition method allows for variation of the local coordinate system on an element-by-element basis with a single orientation definition. For example, if local node number 2 is given as the location of point c and local node number 3 is given as the location of point a, the local -direction is defined to be parallel to the (2, 3) side of the element. By default, the origin (point c) of the local coordinate system is the first node of the element (local node number 1).
| Input File Usage: | *ORIENTATION, NAME=name, DEFINITION=OFFSET TO NODES |
| ABAQUS/CAE Usage: | You cannot define a coordinate system by giving local node numbers in ABAQUS/CAE. |
You can define a coordinate system by specifying an offset from an existing coordinate system.
| Input File Usage: | You cannot define a coordinate system by giving an offset from another coordinate system in the input file. |
| ABAQUS/CAE Usage: | Any module: Tools |
You can define a coordinate system by specifying two edges. The first edge defines the X- or R-axis, and the X–Y or 
plane passes through the second.
| Input File Usage: | You cannot define a coordinate system by giving two edges in the input file. |
| ABAQUS/CAE Usage: | Any module: Tools |
In some cases the simplest way to specify a local system is by means of a user subroutine. User subroutine ORIENT is provided in ABAQUS/Standard. In this case the user subroutine is called each time that an orientation definition is needed. In a model defined in terms of an assembly of part instances, the local directions defined by user subroutine ORIENT must be defined relative to the coordinate system of the assembly.
| Input File Usage: | *ORIENTATION, NAME=name, SYSTEM=USER |
| ABAQUS/CAE Usage: | You can enter the name of an orientation defined in user subroutine ORIENT whenever a user-defined orientation is allowed. |
Because the orientation is independent of the material definition and they can both be referenced in any element property definition, the ability to describe complex structural components (such as laminated composite shells) is quite general and straightforward to use.
An orientation definition can be used as often as needed and with different material or element type definitions; for example, it can be used for different layers of a shell where the orientation is the same.
In ABAQUS/Standard a local rectangular coordinate system for material definitions, material calculations, and output can be defined for continuum and shell elements on an element-by-element basis by using an element property assignment. See “Assigning element properties on an element-by-element basis,” Section 21.1.5, for details.
In large-displacement analysis a user-defined orientation rotates with the average rigid body motion of the material point, the rigid body when the orientation is used with ROTARYI elements, the first node of the joint in JOINTC elements, the pipeline edge for pipe-soil interaction elements, the appropriate surface for contact in ABAQUS/Standard, or the reference node when the orientation is used with coupling constraints. However, when an orientation is defined for spring, dashpot, or gasket elements in ABAQUS/Standard, the local directions always remain fixed in space.
Because the material directions rotate with the average rigid body motion at a material point, using anisotropic elasticity to model a material that is not truly a continuum can give significant errors if shear deformation is large. For example, an individual fiber in a reinforcing belt of a tire can shear relatively easily with respect to fibers in other directions. The fibers rotate with the actual deformation of the material point and not with the average rigid body motion. In this case the anisotropic behavior is better modeled with rebars.
When a user-defined orientation is used with two-dimensional solid elements such as plane stress, plane strain, or torsionless axisymmetric elements, the orientation must redefine only the X- and Y-directions: the third direction must remain unchanged (Z-direction for plane strain and plane stress elements, 
-direction for axisymmetric elements). When a user-defined orientation is used with axisymmetric elements with twist, all three directions can be redefined. For axisymmetric elements, including the CGAX and CAXA families of elements, the global 1-, 2-, and 3-directions are the radial, axial, and hoop directions, respectively. Cylindrical or spherical orientations may be appropriate for axisymmetric elements only if the local -direction is in the global 3-, or hoop, direction.
When a user-defined orientation is used with shell, membrane, or gasket elements or with contact surfaces, you must specify an additional angle of rotation about one of the user-defined axes. The other two orientation axes are rotated by this additional angle. After the rotation ABAQUS follows a cyclic permutation (1, 2, 3) of the axes and projects the axis following the axis for additional rotation onto the contact surface or onto the surface of the element to form the local material 1-direction (or the local material 2-direction for gaskets). The remaining material direction is then defined by the cross product of the element normal and the projected direction. Thus, for example:
If you choose the user-defined 1-axis as the axis for additional rotation, ABAQUS projects the 2-axis onto the element or contact surface. This will be local direction 1 for contact surfaces, shells, and membranes and local direction 2 for gaskets.
ABAQUS takes the positive element or contact surface normal as the local 3-direction for contact surfaces, shells, and membranes and the local 1-direction for gaskets.
ABAQUS computes the local 2-direction (3-direction for gaskets) by taking the cross product of the element or contact surface normal and the local 1-direction (2-direction for gaskets), such that the three local axes form an orthonormal, right-handed local coordinate system.
Figure 2.2.5–3 The local 3-direction (1-direction for gaskets) will be in the same direction as the element or contact surface normal.
As an example, the orientation of the spiral-wound layer of the cylindrical shell shown in Figure 2.2.5–4 would be given by defining a cylindrical coordinate system and then specifying the rotation axis as the 1-axis and giving the rotation angle 
(in degrees). The local 1- and 2-directions for material property specification and material calculations are then those indicated in the figure.
The projected directions are most easily understood when the axis for additional rotation is approximately perpendicular to the element or contact surface.
The orientation of skew rebars in shell, membrane, and surface elements can be defined relative to a user-defined orientation (see “Defining reinforcement,” Section 2.2.3). In this case the local coordinate system is calculated as follows:
ABAQUS finds the user-defined direction (not including the axis for additional rotation) that most closely lies in the plane of the element. This direction is projected onto the element and normalized (so that it is a unit vector).
The axis for additional rotation is made orthogonal to the element to create the local 3-direction. This local 3-direction need not be in the same direction as the element normal.
An orthonormal, right-handed local coordinate system is calculated by taking the cross product of the projected direction and the local 3-direction.
When a user-defined orientation is used to define the tangential slip directions on a surface of a three-dimensional contact pair in ABAQUS/Standard (see “Contact formulation for ABAQUS/Standard contact pairs,” Section 29.2.2), you cannot define points a and b by giving local node numbers (see Figure 2.2.5–1).
For geometrically nonlinear analysis the tangential slip directions of a contact pair rotate with the surface on which the directions were defined initially. These rotated tangential slip directions are further rotated to ensure that the normal vector, computed using the cross product of the rotated tangential slip directions, corresponds to the normal vector on the master surface when the slave node comes into contact.
Arbitrary slip directions can be defined for a “line”-type slave surface defined on three-dimensional beam, truss, or pipe elements. When this surface comes into contact with the master surface during a large-displacement analysis, the slip directions are projected onto the master surface.
When a user-defined orientation is used with laminated shells, 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 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 local direction defined as the axis for additional rotation. If the user-defined orientation directions are not in the surface of the shell, the layer angle is applied 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 23.6.5, and “Using a general shell section to define the section behavior,” Section 23.6.6, for more information.
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 22.1.1, for more information.
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.
See “Beam element cross-section orientation,” Section 23.3.4, for information on defining local material directions for beams, frames, or trusses.
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 18.4.1), 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.
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 25.1.5).
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.
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 28.2.3). In this case you cannot define points a, b, and c by giving local node numbers (see Figure 2.2.5–1).
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 28.3.2). In this case you cannot define points a, b, and c by giving local node numbers (see Figure 2.2.5–1).
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).
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 27.4.3.
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.
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.
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.
