Abaqus/Standard output variable identifiers | ||||||
|
| |||||
ProductsAbaqus/Standard
Notation used in the output variable descriptions
The words .dat, .fil, .odb Field, and .odb History in the output variable's description indicate the availability of the output variable. .dat refers to a data file output selection, .fil refers to a results file output selection, .odbField refers to a field-type output selection to the output database, and .odbHistory refers to a history-type output selection to the output database. 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.
If the word automatic appears after a category name, the variable cannot be requested by name; it will be written to the respective files according to the conditions specified in the text.
Requesting output of components
Variable identifiers of the form ABCn can be used with (ABC1, ABC2, …), where the highest value of n is determined by the type of variable. Similarly, variable identifiers of the form DEF can be used for the ranges of i and j indicated (DEF11, DEF12, ).
Individual components cannot be requested in the results (.fil) file. For postprocessing of a particular component of a variable, request file output for all components of the variable. Output for individual variables can be requested during postprocessing.
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 to the output database are not available for field-type output, with the exception of state, field, and user-defined variables (SDVn, FVn, and UVARMn). 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 field output can be requested within the Visualization module of Abaqus/CAE.
Direction definitions
The direction definitions depend on the variable type.
Direction definitions for element variables
For components of stress, strain, and other tensor quantities 1, 2, and 3 refer to the directions in an orthogonal coordinate system. These directions are global directions for solid elements, surface directions for shell and membrane elements, and axial and transverse directions for beam elements. For finite-membrane-strain shell elements, membrane elements, and continuum elements associated with a local orientation (see Orientations), the local output directions rotate with the average rotation of the element (integral with respect to time of the spin—see Stress rates). Tensor components in these cases are output in the rotating local directions.
In some cases the local output directions may differ from one integration point to the next within an element. Abaqus/Standard does not take this variation into account when extrapolating output variables to the nodes, which affects output such as element quantities averaged at the nodes or contour plots of individual tensor components. Invariant quantities at the integration points will not be influenced by the local output directions.
You can control writing the local directions to the output database file or to the results file (see Specifying the directions for element output in Abaqus/Standard and Abaqus/Explicit and Output of local directions to the results file). By default, the local directions are written to the output database for all frames that include element field output. The local (material) directions (averaged at the nodes) can be visualized in Abaqus/CAE by selecting in the Visualization module. The directions can be printed to the data file by using user subroutine UVARM.
Direction definitions for equivalent rigid body variables
For all equivalent rigid body variables 1, 2, and 3 refer to global directions.
Direction definitions for nodal variables
For nodal variables 1, 2, and 3 are global directions (1=X, 2=Y, and 3=Z; or for axisymmetric elements, 1=r and 2=z). If a local coordinate system is defined at a node (see Transformed coordinate systems), you can specify whether output to the data or results file of vector-valued quantities at these nodes is in the local or global system (see Specifying the directions for nodal output). By default, nodal output is written to the data file in the local system, whereas it is written to the results file in the global system (since this is more convenient for postprocessing).
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
You need to be aware of limitations that may be encountered when distributed load output is requested.
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/Standard User Subroutines) are not displayed, except for the variables FILMCOEF and SINKTEMP.
Distributed load output with modal procedures
For modal procedures only the magnitude of the load is written to the output database.
Strain output
The total strain E is composed of the elastic strain EE, the inelastic strain IE, and the thermal strain THE. The inelastic strain IE consists of the plastic strain PE and the creep strain CE.
For geometrically nonlinear analysis Abaqus/Standard makes it possible to output different strain measures as well as elastic and various inelastic strains. The various total strain measures (integrated strain measure E, nominal strain measure NE, and logarithmic strain measure LE) are described in Conventions. The default strain measure for output to the data (.dat) and results (.fil) files is E. However, for geometrically nonlinear analysis using element formulations that support finite strains, E is not available for output to the output database (.odb) file, and LE is the default strain measure.
Temperature output
In Abaqus temperature can either be a field variable (stress analysis, mass diffusion, …) or a degree of freedom (heat transfer analysis, fully coupled temperature-displacement analysis, …). For any analysis that involves temperature, you can request the temperature either at nodes (variable NT) or in elements (variable TEMP). If element temperature output is requested at the nodes, the integration point values are extrapolated and, if requested, averaged. These extrapolated values are generally not as accurate as the nodal temperatures themselves. An exception to this is adiabatic analysis, in which the element temperatures change due to plastic heat generation but the nodal temperatures are not updated. In that case the current nodal temperatures are obtained only if element temperature output is requested at the nodes.
For continuum elements there is only one temperature value per node (NT11). For shells and beams more than one temperature is available for each node (NT11, NT12, …) since a temperature gradient can exist through the thickness of a shell or across the cross-section of a beam. In general, variables NT12, NT13, etc. contain temperature values. However, when temperature is defined by specifying temperature gradients, nodal temperatures for a given section point can be obtained only by using the variable TEMP. See Specifying temperature and field variables and Specifying temperature and field variables for discussions on specifying temperatures in beams and shells.
Principal value output
Output of the principal values can be requested for stresses, strains, and other material tensors. Either all principal values or the minimum, maximum, or intermediate values can be obtained. All principal values of tensor ABC are obtained with the request ABCP. The minimum, intermediate, and maximum principal values are obtained with the requests ABCP1, ABCP2, and ABCP3.
For three-dimensional, (generalized) plane strain, and axisymmetric elements all three principal values are obtained. For plane stress, membrane, and shell elements, the out-of-plane principal value cannot be requested for history-type output. For field-type output, Abaqus/CAE always reports the out-of-plane principal value as zero. Principal values cannot be obtained for truss elements or for any beam elements other than the three-dimensional beam elements with torsional shear stresses.
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 explicitly requested 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 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.
For plane stress, membrane, and shell elements, only the in-plane tensor components (11, 22, and 12 components) are stored by Abaqus/Standard. The out-of-plane direct component for stress (S33) is reported as zero to the output database as expected, and the out-of-plane component of strain (E33) is reported as zero even though it is not. This is because the thickness direction is computed based on section properties rather than at the material level. The out-of-plane components can be requested for field-type output and cannot be requested for history-type output. The out-of-plane stress components are not reported to the data (.dat) file or to the results (.fil) file.
For three-dimensional beam elements with torsional shear stresses, only the axial and the torsional components (the 11 and 12 components) are stored by Abaqus/Standard. The other direct component (the 22 component) is reported as zero for field-type output and cannot be requested for history-type output.
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 nonzero values.