<!-- source-page: 761 -->

<table><tr><td rowspan="2">Identifier</td><td rowspan="2">.dat</td><td rowspan="2">.fil</td><td colspan="2">.odb</td><td rowspan="2">Description</td></tr><tr><td>Field</td><td>History</td></tr><tr><td colspan="6">All analysis types</td></tr><tr><td>SOAREA</td><td>●</td><td>●</td><td></td><td>●</td><td>Area of the defined section.</td></tr><tr><td colspan="6">Stress/displacement analysis</td></tr><tr><td>SOF</td><td>●</td><td>●</td><td></td><td>●</td><td>Total force in the section.</td></tr><tr><td>SOM</td><td>●</td><td>●</td><td></td><td>●</td><td>Total moment in the section.</td></tr><tr><td>SOCF</td><td>●</td><td>●</td><td></td><td>●</td><td>Center of the total force in the section.</td></tr><tr><td colspan="6">Heat transfer analysis</td></tr><tr><td>SOH</td><td>●</td><td>●</td><td></td><td>●</td><td>Total heat flux associated with the section.</td></tr><tr><td colspan="6">Electrical analysis</td></tr><tr><td>SOE</td><td>●</td><td>●</td><td></td><td>●</td><td>Total current associated with the section.</td></tr><tr><td colspan="6">Mass diffusion analysis</td></tr><tr><td>SOD</td><td>●</td><td>●</td><td></td><td>●</td><td>Total mass flow associated with the section.</td></tr><tr><td colspan="6">Coupled pore fluid diffusion-stress analysis</td></tr><tr><td>SOP</td><td>●</td><td>●</td><td></td><td>●</td><td>Total pore fluid volume flux associated with the section.</td></tr></table>

# Whole and partial model variables

The output variables listed below are available for part of the model as well as the whole model.

Identifier .dat .fil .odb Description Field History

# Adaptive mesh domains

The following variable is available only for adaptive domains (see “Defining ALE adaptive mesh domains in Abaqus/Standard,” Section 12.2.6).

VOLC Change in area or change in volume of an element set solely due to adaptive meshing.

# Equivalent rigid body motion variables

You can request equivalent rigid body motion whole element set variable output to the data, results, or output database file (see “Element output” in “Output to the data and results files,” Section 4.1.2, and

<!-- source-page: 762 -->

Identifier .dat .fil .odb Description Field History

“Element output” in “Output to the output database,” Section 4.1.3). The variables listed are available only for implicit dynamic analyses using direct integration except where indicated.

<table><tr><td>XC</td><td>•</td><td>•</td><td>•</td><td>Current coordinates of the center of mass for the entire set or the entire model. Not available for eigenfrequency extraction, eigenvalue buckling prediction, complex eigenfrequency extraction, or linear dynamics procedures. Available also for static analyses but only from the output database.</td></tr><tr><td>XCn</td><td>•</td><td></td><td>•</td><td>Coordinate n of the center of mass for the entire set or the entire model (n = 1, 2, 3).</td></tr><tr><td>UC</td><td>•</td><td>•</td><td>•</td><td>Current displacement of the center of mass for the entire set or the entire model. Available also for static analyses but only from the output database.</td></tr><tr><td>UCn</td><td>•</td><td></td><td>•</td><td>Displacement component n of the center of mass for the entire set or the entire model (n = 1, 2, 3).</td></tr><tr><td>URCn</td><td>•</td><td></td><td>•</td><td>Rotation component n of the center of mass for the entire set or the entire model (n = 1, 2, 3).</td></tr><tr><td>VC</td><td>•</td><td>•</td><td>•</td><td>Equivalent rigid body velocity components summed over the entire set or the entire model.</td></tr><tr><td>VCn</td><td>•</td><td></td><td>•</td><td>Component n of the equivalent rigid body velocity summed over the entire set or the entire model (n = 1, 2, 3).</td></tr><tr><td>VRCn</td><td>•</td><td></td><td>•</td><td>Component n of the equivalent rigid body angular velocity summed over the entire set or the entire model (n = 1, 2, 3).</td></tr><tr><td>HC</td><td>•</td><td>•</td><td>•</td><td>Current angular momentum about the center of mass for the entire set or the entire model.</td></tr><tr><td>HCn</td><td>•</td><td></td><td>•</td><td>Component n of the angular momentum about the center of mass for the entire set or the entire model (n = 1, 2, 3).</td></tr><tr><td>HO</td><td>•</td><td>•</td><td>•</td><td>Current angular momentum about the origin for the entire set or the entire model.</td></tr><tr><td>HOn</td><td>•</td><td></td><td>•</td><td>Component n of the angular momentum about the origin for the entire set or the entire model (n = 1, 2, 3).</td></tr><tr><td>RI</td><td>•</td><td>•</td><td>•</td><td>Current rotary inertia about the origin of the entire set or the entire model. Not available for eigenfrequency</td></tr></table>

<!-- source-page: 763 -->

<table><tr><td>Identifier</td><td>.dat</td><td>.fil</td><td>.odb</td><td>Description</td></tr><tr><td></td><td></td><td></td><td>Field History</td><td></td></tr><tr><td></td><td></td><td></td><td></td><td>extraction, eigenvalue buckling prediction, complex eigenfrequency extraction, or linear dynamics procedures. Available also for static analyses but only from the output database.</td></tr><tr><td>RIij</td><td>•</td><td></td><td>•</td><td>ij-component of the rotary inertia about the origin of the entire set or the entire model (i ≤ j ≤ 3).</td></tr><tr><td>MASS</td><td>•</td><td>•</td><td>•</td><td>Current mass of the entire set or the entire model. Available also for static analyses but only from the output database.</td></tr><tr><td>VOL</td><td>•</td><td>•</td><td>•</td><td>Current volume of the entire set or the entire model. Available also for static analyses but only from the output database. (Available only for continuum and structural elements that do not use general beam or shell section definitions.)</td></tr></table>

# Inertia relief output variables

You can request inertia relief whole model variable output to the data or output database file (see “Element output” in “Output to the data and results files,” Section 4.1.2, and “Element output” in “Output to the output database,” Section 4.1.3). Since these variables have unique values for the entire model, the variable output is independent of the specified region. The variables listed are available only for those analyses that include inertia relief loading (see “Inertia relief,” Section 11.1.1).

<table><tr><td>IRX</td><td>•</td><td>•</td><td>Current coordinates of the reference point.</td></tr><tr><td>IRXn</td><td>•</td><td>•</td><td>Coordinate n of the reference point (n = 1, 2, 3).</td></tr><tr><td>IRA</td><td>•</td><td>•</td><td>Equivalent rigid body acceleration components.</td></tr><tr><td>IRAn</td><td>•</td><td>•</td><td>Component n of the equivalent rigid body acceleration (n = 1, 2, 3).</td></tr><tr><td>IRARn</td><td>•</td><td>•</td><td>Component n of the equivalent rigid body angular acceleration with respect to the reference point (n = 1, 2, 3).</td></tr><tr><td>IRF</td><td>•</td><td>•</td><td>Inertia relief load corresponding to the equivalent rigid body acceleration.</td></tr><tr><td>IRFn</td><td>•</td><td>•</td><td>Component n of the inertia relief load corresponding to the equivalent rigid body acceleration (n = 1, 2, 3).</td></tr><tr><td>IRMn</td><td>•</td><td>•</td><td>Component n of the inertia relief moment corresponding to the equivalent rigid body angular acceleration with respect to the reference point (n = 1, 2, 3).</td></tr></table>

<!-- source-page: 764 -->

<table><tr><td rowspan="2">Identifier</td><td rowspan="2">.dat</td><td rowspan="2">.fil</td><td colspan="2">.odb</td><td rowspan="2">Description</td></tr><tr><td>Field</td><td>History</td></tr><tr><td>IRRI</td><td>•</td><td></td><td></td><td>•</td><td>Rotary inertia about the reference point.</td></tr><tr><td>IRRIij</td><td>•</td><td></td><td></td><td>•</td><td>ij-component of the rotary inertia about the reference point (i ≤ j ≤ 3).</td></tr><tr><td>IRMASS</td><td>•</td><td></td><td></td><td>•</td><td>Whole model mass.</td></tr></table>

# Mass diffusion analysis

You can request variable output from a mass diffusion analysis (“Mass diffusion analysis,” Section 6.9.1) to the data, results, or output database file (see “Element output” in “Output to the data and results files,” Section 4.1.2, and “Element output” in “Output to the output database,” Section 4.1.3). If you specify an output region, the variable is calculated over the user-specified region. If you do not specify an output region, the variable is calculated as the total over the entire model.

SOL Amount of solute in an element set, calculated as the sum of ESOL (amount of solute in each element) over all the elements in the set.

# Analyses with time-dependent material behavior

CRPTIME Creep time, which is equal to the total time in procedures with time-dependent material behavior (see “Rate-dependent plasticity: creep and swelling,” Section 23.2.4).

# Eigenvalue extraction

The following variables are output automatically during a frequency extraction analysis (“Natural frequency extraction,” Section 6.3.5).

<table><tr><td>EIGVAL</td><td>○</td><td>○</td><td>Eigenvalues.</td></tr><tr><td>EIGFREQ</td><td>○</td><td>○</td><td>Eigenfrequencies.</td></tr><tr><td>GM</td><td>○</td><td>○</td><td>Generalized masses.</td></tr><tr><td>CD</td><td>○</td><td>○</td><td>Composite damping factors.</td></tr><tr><td>PFn</td><td>○</td><td>○</td><td>Modal participation factors 1–7 (n = 1,2,3 corresponding to displacements, n = 4,5,6 for the rotations, and n = 7 for acoustic pressure).</td></tr><tr><td>EMn</td><td>○</td><td>○</td><td>Modal effective masses 1–7 (n = 1,2,3 corresponding to displacements, n = 4,5,6 for the rotations, and n = 7 for acoustic pressure).</td></tr></table>

<!-- source-page: 765 -->

Identifier .dat .fil .odb Description

# Field History

# Complex eigenvalue extraction

The following variables are output automatically during a complex frequency extraction analysis (“Complex eigenvalue extraction,” Section 6.3.6).

<table><tr><td>EIGREAL</td><td>○</td><td>○</td><td>Real parts of the eigenvalues.</td></tr><tr><td>EIGIMAG</td><td>○</td><td>○</td><td>Imaginary parts of the eigenvalues.</td></tr><tr><td>EIGFREQ</td><td>○</td><td>○</td><td>Eigenfrequencies.</td></tr><tr><td>DAMPRATIO</td><td>○</td><td>○</td><td>Damping ratios.</td></tr></table>

# Total energy output quantities

If the following whole model variables are relevant for a particular analysis, you can request them as output to the data, results, or output database file (see “Total energy output” in “Output to the data and results files,” Section 4.1.2, and “Total energy output” in “Output to the output database,” Section 4.1.3). If you do not specify an output region, whole model variables are calculated. When you specify an output region, the relevant energy totals are calculated over the user-specified region.

These variables are not available for eigenvalue buckling prediction, eigenfrequency extraction, or complex frequency extraction analysis. You cannot specify an output region for modal dynamic, random response, response spectrum, or steady-state dynamic analysis.

See “Energy balance,” Section 1.5.5 of the Abaqus Theory Guide and “Energy computations in a contact analysis,” Section 1.1.25 of the Abaqus Example Problems Guide, for details of the energy definitions. In steady-state dynamics all energy quantities are net per-cycle values, unless otherwise noted.

<table><tr><td>ALLAE</td><td>○</td><td>○</td><td>•</td><td>“Artificial” strain energy associated with constraints used to remove singular modes (such as hourglass control), and with constraints used to make the drill rotation follow the in-plane rotation of the shell elements.</td></tr><tr><td>ALLCCDW</td><td>○</td><td></td><td>•</td><td>Contact constraint discontinuity work.</td></tr><tr><td>ALLCCEN</td><td>○</td><td></td><td>•</td><td>Contact constraint elastic energy in normal direction due to penalty constraint enforcement.</td></tr><tr><td>ALLCCET</td><td>○</td><td></td><td>•</td><td>Contact constraint elastic energy in tangential direction due to friction penalty constraint enforcement.</td></tr><tr><td>ALLCCE</td><td>○</td><td></td><td>•</td><td>The sum of ALLCCEN and ALLCCET.</td></tr><tr><td>ALLCCSDN</td><td>○</td><td></td><td>•</td><td>Contact constraint stabilization dissipation in normal direction.</td></tr></table>

<!-- source-page: 766 -->

<table><tr><td rowspan="2">Identifier</td><td rowspan="2">.dat</td><td rowspan="2">.fil</td><td colspan="2">.odb</td><td rowspan="2">Description</td></tr><tr><td>Field</td><td>History</td></tr><tr><td>ALLCCSDT</td><td>○</td><td></td><td></td><td>●</td><td>Contact constraint stabilization dissipation in tangential direction.</td></tr><tr><td>ALLCCSD</td><td>○</td><td></td><td></td><td>●</td><td>The sum of ALLCCSDN and ALLCCSDT.</td></tr><tr><td>ALLCD</td><td>○</td><td>○</td><td></td><td>●</td><td>Energy dissipated by creep, swelling, viscoelasticity, and energy associated with viscous regularization for cohesive elements and cohesive contact.</td></tr><tr><td>ALLEE</td><td>○</td><td>○</td><td></td><td>●</td><td>Electrostatic energy.</td></tr><tr><td>ALLFD</td><td>○</td><td>○</td><td></td><td>●</td><td>Total energy dissipated through frictional effects. (Available only for the whole model.)</td></tr><tr><td>ALLIE</td><td>○</td><td>○</td><td></td><td>●</td><td>Total strain energy. (ALLIE = ALLSE + ALLPD + ALLCD + ALLAE + ALLQB + ALLEE + ALLDMD.)</td></tr><tr><td>ALLJD</td><td>○</td><td>○</td><td></td><td>●</td><td>Electrical energy dissipated due to flow of electrical current.</td></tr><tr><td>ALLKE</td><td>○</td><td>○</td><td></td><td>●</td><td>Kinetic energy. In steady-state dynamic analysis this is the cyclic mean value.</td></tr><tr><td>ALLKL</td><td>○</td><td>○</td><td></td><td>●</td><td>Loss of kinetic energy at impact. (Available only for the whole model.)</td></tr><tr><td>ALLPD</td><td>○</td><td>○</td><td></td><td>●</td><td>Energy dissipated by rate-independent and rate-dependent plastic deformation.</td></tr><tr><td>ALLQB</td><td>○</td><td>○</td><td></td><td>●</td><td>Energy dissipated through quiet boundaries (infinite elements). (Available only for the whole model.)</td></tr><tr><td>ALLSD</td><td>○</td><td>○</td><td></td><td>●</td><td>Energy dissipated by automatic stabilization. This includes both volumetric static stabilization and automatic approach of contact pairs (the latter part included only for the whole model).</td></tr><tr><td>ALLSE</td><td>○</td><td>○</td><td></td><td>●</td><td>Recoverable strain energy. In steady-state dynamic analysis this is the cyclic mean value.</td></tr><tr><td>ALLVD</td><td>○</td><td>○</td><td></td><td>●</td><td>Energy dissipated by viscous effects including viscous regularization (except for cohesive elements and cohesive contact), not inclusive of energy dissipated by automatic stabilization and viscoelasticity.</td></tr><tr><td>ALLDMD</td><td>○</td><td>○</td><td></td><td>●</td><td>Energy dissipated by damage.</td></tr><tr><td>ALLWK</td><td>○</td><td>○</td><td></td><td>●</td><td>External work. (Available only for the whole model.)</td></tr><tr><td>ETOTAL</td><td>○</td><td>○</td><td></td><td>●</td><td>Total energy balance (available only for the whole model). (ETOTAL = ALLKE + ALLIE + ALLVD + ALLSD + ALLKL + ALLFD + ALLJD + ALLCCE - ALLWK - ALLCCDW.)</td></tr></table>

<!-- source-page: 767 -->

# Solution-dependent amplitude variables

Solution-dependent amplitude variables are given automatically with any file output or output database request.

<table><tr><td rowspan="2">Identifier</td><td rowspan="2">.dat</td><td rowspan="2">.fil</td><td colspan="2">.odb</td><td rowspan="2">Description</td></tr><tr><td>Field</td><td>History</td></tr><tr><td>LPF</td><td></td><td>○</td><td></td><td>○</td><td>Load proportionality factor in a static Riks analysis.</td></tr><tr><td>AMPCU</td><td></td><td>○</td><td></td><td>○</td><td>Current value of the solution-dependent amplitude.</td></tr><tr><td>RATIO</td><td></td><td>○</td><td></td><td>○</td><td>Current maximum ratio of creep strain rate and target creep strain rate.</td></tr></table>

# Structural optimization variables

Structural optimization output variables are requested by the Optimization module during each design cycle. For more information, see Chapter 13, “Optimization Techniques.”

Identifier .dat .fil .odb Description Field History

# Toplogy optimization

The following variable is output automatically during topology optimization (see “Topology optimization” in “Structural optimization: overview,” Section 13.1.1).

MAT\_PROP\_NORMALIZED Element-based normalized material value.

# Shape optimization

The following variables are output automatically during shape optimization (see “Shape optimization” in “Structural optimization: overview,” Section 13.1.1).

<table><tr><td>CTRL_INPUT</td><td>○</td><td>The value of the objective function at each node.</td></tr><tr><td>DISP_OPT_VAL</td><td>○</td><td>The value of the shape optimization displacement.</td></tr><tr><td>DISP_OPT</td><td>○</td><td>A vector representing the shape optimization displacement.</td></tr></table>

# Sizing optimization

The following variables are output automatically during sizing optimization (see “Sizing optimization” in “Structural optimization: overview,” Section 13.1.1).

<table><tr><td>THICKNESS</td><td>○</td><td>The value of the shell thickness.</td></tr><tr><td>DELTA_THICKNESS</td><td>○</td><td>The change in shell thickness.</td></tr></table>

<!-- source-page: 768 -->

Identifier

.dat .fil

.odb

Description

Field History

# Bead optimization

The following variables are output automatically during bead optimization (see “Bead optimization” in “Structural optimization: overview,” Section 13.1.1).

DISP\_NORMAL\_VAL

0

The value of the bead optimization displacement along the node normal vector.

DISP\_OPT\_VAL

0

The value of the bead optimization displacement.

DISP\_OPT

0

A vector representing the bead optimization displacement.

<!-- source-page: 769 -->

# 4.2.2 Abaqus/Explicit OUTPUT VARIABLE IDENTIFIERS

Product: Abaqus/Explicit

# References

• “Output,” Section 4.1.1   
• “Output to the data and results files,” Section 4.1.2   
• “Output to the output database,” Section 4.1.3

# Overview

Except for the information in the status file, results can be obtained from Abaqus/Explicit only by postprocessing.

The tables in this section list all of the output variables that are available in Abaqus/Explicit. These output variables can be requested for output to the results (.fil) file (see “Output to the data and results files,” Section 4.1.2) or as either field- or history-type output to the output database (.odb) file (see “Output to the output database,” Section 4.1.3). In general, output variables that can be requested as fieldor history-type output to an output database in ODB format can also be requested as output in SIM format (see “The output database” in “Output,” Section 4.1.1). When the output variables are requested for output to the results file, Abaqus/Explicit will first output these variables to the selected results (.sel) file and will then convert the selected results file to the results file after the analysis completes.

# Symbols used in the tables

The availability of the various output variable identifiers is defined by a in the columns of the table, under the following headings:

.fil

means that the identifier can be used as a results file output selection.

.odb Field

means that the identifier can be used as a field-type output selection to the output database.

.odb History

means that the identifier can be used as a history-type output selection to the output database.

# Direction definitions

The direction definitions depend on the variable type.

<!-- source-page: 770 -->

# 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,” Section 2.2.5) 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,” Section 2.1.5), 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,” Section 2.5.1) 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,” Section 34.4. However, contributions to these loads defined through user subroutines (see “Abaqus/Explicit subroutines,” Section 1.2 of the Abaqus User Subroutines Reference Guide) 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 historytype 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.
