Abaqus/Explicit output variable identifiers | ||||||
|
| |||||
Products Abaqus/Explicit
Notation used in the output variable descriptions
The words .fil, .odb Field, and .odb History in the output variable's description indicate the availability of the output variable. .fil refers to output to the results file. The output variable can be written to the respective file if the word yes appears after the category name; no means that the variable is not available to that file.
Direction definitions
The direction definitions depend on the variable type.
Direction definitions for element variables
For components of stress, strain, and similar material variables, 1, 2, and 3 refer to the directions in an orthogonal coordinate system. These are global directions for solid elements, surface directions for shell and membrane elements, and axial and transverse directions for beam and pipe elements. However, if a local orientation (Orientations) is associated with the elements for which output is being requested, 1, 2, and 3 are local directions.
Direction definitions for nodal variables
For nodal variables, 1, 2, and 3 refer to the global directions (1=X, 2=Y, 3=Z except for axisymmetric elements, in which case 1=R, 2=Z). Even if a local coordinate system has been defined at a node (Transformed coordinate systems), the data in the results file and the selected results file are still output in the global directions.
If nodal field output is requested for a node that has a local coordinate system defined, a quaternion representing the rotation from the global directions is written to the output database. Abaqus/CAE automatically uses this quaternion to transform the nodal results into the local directions. Nodal history data written to the output database are always stored in the global directions.
Direction definitions for integrated variables
For components of total force, total moment, and similar variables obtained through integration over a surface, the directions 1, 2, and 3 refer to directions in an orthogonal coordinate system. A fixed global coordinate system is used if the surface is specified directly for the integrated output request. If the surface is identified by an integrated output section definition (see Integrated output section definition) that is associated with the integrated output request, a local coordinate system in the initial configuration can be specified and can translate or rotate with the deformation.
Distributed load output and user subroutines
Output can be requested for many of the distributed loads discussed in Loads. However, contributions to these loads defined through user subroutines (see Abaqus/Explicit User Subroutines) are not displayed.
Principal value output
Output of the principal values can be requested for stresses, logarithmic strains, and nominal strains. Either all principal values or the minimum, intermediate, or maximum values can be obtained. All principal values of tensor ABC are obtained with the request ABCP, and the minimum, intermediate, and maximum principal values are obtained with the requests ABCP1, ABCP2, and ABCP3, respectively. For three-dimensional, plane strain, and axisymmetric elements all three principal values are obtained. For plane stress, membrane, and shell elements only the in-plane principal values are obtained for history-type output, and the out-of-plane principal value cannot be requested. For field-type output, all three principal values are obtained through Abaqus/CAE. Principal values cannot be obtained for beam, pipe, and truss elements, and principal values of plastic strains cannot be requested.
If a principal value or an invariant is requested for field-type output, the output request is replaced with an output request for the components of the corresponding tensor. Abaqus/CAE calculates all principal values and invariants from these components. If a principal value is desired as history-type output, it must be requested explicitly since Abaqus/CAE does no calculations on history data.
Tensor output
Tensor variables that are written to the output database as field-type output are written as components in either the default directions defined by the convention given in Orientations (global directions for solid elements, surface directions for shell and membrane elements, and axial and transverse directions for beam and pipe elements), or the user-defined local system. Abaqus/CAE calculates all principal values and invariants from these components. See Writing field output data, for a description of the different types of tensor variables.
The components for tensor variables are written to the output database in single precision. Therefore, a small amount of precision roundoff error may occur when calculating the variables' principal values. Such roundoff error may be observed, for example, when analytically zero values are calculated as relatively small yet nonzero values.
Requesting output of components
Individual components of variables can be requested as history-type output in the output database for X–Y plotting in Abaqus/CAE. Individual component requests are not available for field-type output. If a particular component is desired for contouring in Abaqus/CAE, request field output of the generic variable (e.g., S for stress). Output for individual components of this field output can be requested within the Visualization module of Abaqus/CAE.