<!-- source-page: 661 -->

<table><tr><td>Procedure type</td><td>Preselected element variables (field; history for Abaqus/CFD)</td><td>Preselected nodal and surface variables (field)</td><td>Preselected energy variables (history)</td></tr><tr><td>Direct cyclic</td><td>S, E, PE, PEEQ, PEMAG</td><td>U, RF, CF</td><td>ALLAE, ALLCCDW, ALLCCE, ALLCCEN, ALLCCET, ALLCCSD, ALLCCSDN, ALLCCSDT, ALLCD, ALLFD, ALLIE, ALLKE, ALLPD, ALLSE, ALLVD, ALLDMD, ALLWK, ALLKL, ALLQB, ALLEE, ALLJD, ALLSD, ETOTAL</td></tr><tr><td>Direct-integration implicit dynamic (with an output frequency of 10)</td><td>S, E, PE, PEEQ, PEMAG</td><td>U, V, A, RF, CF, CSTRESS, CDISP</td><td>ALLAE, ALLCCDW, ALLCCE, ALLCCEN, ALLCCET, ALLCCSD, ALLCCSDN, ALLCCSDT, ALLCD, ALLFD, ALLIE, ALLKE, ALLPD, ALLSE, ALLVD, ALLDMD, ALLWK, ALLKL, ALLQB, ALLEE, ALLJD, ALLSD, ETOTAL</td></tr><tr><td>Direct-solution steady-state dynamic</td><td>S, E</td><td>U, V, A, RF, CF</td><td>ALLKE, ALLSE, ALLVD, ALLWK</td></tr><tr><td>Eigenfrequency extraction</td><td>none</td><td>U</td><td>none</td></tr><tr><td>Eigenvalue buckling prediction</td><td>none</td><td>U</td><td>none</td></tr></table>

<!-- source-page: 662 -->

<table><tr><td>Procedure type</td><td>Preselected element variables (field; history for Abaqus/CFD)</td><td>Preselected nodal and surface variables (field)</td><td>Preselected energy variables (history)</td></tr><tr><td>Explicit dynamic</td><td>S, LE, PE, PEEQ, EVF, SVAVG, PEAVG, PEEQVAVG</td><td>U, V, A, RF, CSTRESS</td><td>ALLKE, ALLSE, ALLWK, ALLPD, ALLCD, ALLVD, ALLDMD, ALLAE, ALLIE, ALLFD, ETOTAL</td></tr><tr><td>Fully coupled thermal-electrical-structural in Abaqus/Standard</td><td>S, E, PE, PEEQ, PEMAG, HFL, EPG</td><td>U, RF, CF, NT, RFL, CSTRESS, CDISP, EPOT</td><td>ALLAE, ALLCCDW, ALLCCE, ALLCCEN, ALLCCET, ALLCCSD, ALLCCSDN, ALLCCSDT, ALLCD, ALLFD, ALLIE, ALLKE, ALLPD, ALLSE, ALLVD, ALLDMD, ALLWK, ALLKL, ALLQB, ALLEE, ALLJD, ALLSD, ETOTAL</td></tr><tr><td>Fully coupled thermal-stress in Abaqus/Standard</td><td>S, E, PE, PEEQ, PEMAG, HFL</td><td>U, RF, CF, NT, RFL, CSTRESS, CDISP</td><td>ALLAE, ALLCCDW, ALLCCE, ALLCCEN, ALLCCET, ALLCCSD, ALLCCSDN, ALLCCSDT, ALLCD, ALLFD, ALLIE, ALLKE, ALLPD, ALLSE, ALLVD, ALLDMD, ALLWK, ALLKL, ALLQB, ALLEE, ALLJD, ALLSD, ETOTAL</td></tr></table>

<!-- source-page: 663 -->

<table><tr><td>Procedure type</td><td>Preselected element variables (field; history for Abaqus/CFD)</td><td>Preselected nodal and surface variables (field)</td><td>Preselected energy variables (history)</td></tr><tr><td>Fully coupled thermal-stress in Abaqus/Explicit</td><td>S, LE, PE, PEEQ, HFL</td><td>U, V, A, RF, CSTRESS, NT, RFL</td><td>ALLKE, ALLSE, ALLWK, ALLPD, ALLCD, ALLVD, ALLDMD, ALLAE, ALLIE, ALLFD, ALLIHE, ALLHF, ETOTAL</td></tr><tr><td>Geostatic stress field</td><td>S, E, POR, SAT, VOIDR</td><td>U, RF, CF, CSTRESS, CDISP</td><td>ALLAE, ALLCCDW, ALLCCE, ALLCCEN, ALLCCET, ALLCCSD, ALLCCSDN, ALLCCSDT, ALLCD, ALLFD, ALLIE, ALLKE, ALLPD, ALLSE, ALLVD, ALLDMD, ALLWK, ALLKL, ALLQB, ALLEE, ALLJD, ALLSD, ETOTAL</td></tr><tr><td>Heat transfer</td><td>HFL</td><td>NT, RFL</td><td>none</td></tr><tr><td>Incompressible fluid dynamics in Abaqus/CFD</td><td>V, PRESSURE, TEMP, TURBNU</td><td>U, V, PRESSURE, TEMP, TURBNU</td><td>none</td></tr><tr><td>Linear static perturbation</td><td>S, E</td><td>U, RF, CF</td><td>ALLAE, ALLCCDW, ALLCCE, ALLCCEN, ALLCCET, ALLCCSD, ALLCCSDN, ALLCCSDT, ALLCD, ALLFD, ALLIE, ALLKE, ALLPD, ALLSE, ALLVD, ALLDMD, ALLWK, ALLKL, ALLQB, ALLEE, ALLJD, ALLSD, ETOTAL</td></tr><tr><td>Mass diffusion</td><td>CONC, MFL</td><td>NNC, RFL</td><td>none</td></tr></table>

<!-- source-page: 664 -->

<table><tr><td>Procedure type</td><td>Preselected element variables (field; history for Abaqus/CFD)</td><td>Preselected nodal and surface variables (field)</td><td>Preselected energy variables (history)</td></tr><tr><td>Modal dynamic (with an output frequency of 10)</td><td>S, E</td><td>U, V, A, RF, CF</td><td>ALLAE, ALLCD, ALLFD, ALLIE, ALLKE, ALLPD, ALLSE, ALLVD, ALLDMD, ALLWK, ALLKL, ALLQB, ALLEE, ALLJD, ALLSD, ETOTAL</td></tr><tr><td>SIM-based modal dynamic</td><td>none</td><td>none</td><td>none</td></tr><tr><td>Quasi-static</td><td>S, E, PE, PEEQ, PEMAG, CE, CEEQ, CEMAG</td><td>U, RF, CF, CSTRESS, CDISP</td><td>ALLAE, ALLCCDW, ALLCCE, ALLCCEN, ALLCCET, ALLCCSD, ALLCCSDN, ALLCCSDT, ALLCD, ALLFD, ALLIE, ALLKE, ALLPD, ALLSE, ALLVD, ALLDMD, ALLWK, ALLKL, ALLQB, ALLEE, ALLJD, ALLSD, ETOTAL</td></tr><tr><td>Random response</td><td>S, E</td><td>U, V, A</td><td>none</td></tr><tr><td>Response spectrum</td><td>S, E</td><td>U, RF, CF</td><td>ALLKE, ALLSE, ALLWK</td></tr></table>

<!-- source-page: 665 -->

<table><tr><td>Procedure type</td><td>Preselected element variables (field; history for Abaqus/CFD)</td><td>Preselected nodal and surface variables (field)</td><td>Preselected energy variables (history)</td></tr><tr><td>Static</td><td>S, E, PE, PEEQ, PEMAG</td><td>U, RF, CF, CSTRESS, CDISP</td><td>ALLAE, ALLCCDW, ALLCCE, ALLCCEN, ALLCCET, ALLCCSD, ALLCCSDN, ALLCCSDT, ALLCD, ALLFD, ALLIE, ALLKE, ALLPD, ALLSE, ALLVD, ALLDMD, ALLWK, ALLKL, ALLQB, ALLEE, ALLJD, ALLSD, ETOTAL</td></tr><tr><td>Steady-state dynamic</td><td>S, E</td><td>U, V, A, RF, CF</td><td>ALLKE, ALLSE, ALLWK</td></tr><tr><td>SIM-based steady-state dynamic</td><td>none</td><td>none</td><td>none</td></tr><tr><td>Steady-state transport</td><td>S, E</td><td>U, RF, CF, CSTRESS, CDISP</td><td>ALLAE, ALLCCDW, ALLCCE, ALLCCEN, ALLCCET, ALLCCSD, ALLCCSDN, ALLCCSDT, ALLCD, ALLFD, ALLIE, ALLKE, ALLPD, ALLSE, ALLVD, ALLDMD, ALLWK, ALLKL, ALLQB, ALLEE, ALLJD, ALLSD, ETOTAL</td></tr><tr><td>Subspace-based steady-state dynamic</td><td>S, E</td><td>U, V, A, RF, CF</td><td>ALLKE, ALLSE, ALLVD, ALLWK</td></tr></table>

# Requesting all variables applicable to the current procedure and material type in Abaqus/Standard and Abaqus/Explicit

You can request all variables applicable to the current procedure and material type. Any individual output requests for specific variable types are ignored in this case.

<!-- source-page: 666 -->

<table><tr><td>Input File Usage:</td><td>Use one of the following options:*OUTPUT, FIELD, VARIABLE=ALL*OUTPUT, HISTORY, VARIABLE=ALL</td></tr><tr><td>Abaqus/CAE Usage:</td><td>Step module: field or history output request editor: All</td></tr></table>

# Default output

In Abaqus/Standard and Abaqus/Explicit, if no output database requests are specified, the preselected field and history output variables are written automatically to the output database. In Abaqus/Standard the default variables are written at every increment for both field and history output for all procedure types except dynamic and modal dynamic analyses; the default frequency for field and history output for these procedure types is every 10 increments. In Abaqus/Explicit the default variables are written at 20 intervals for field output and 200 intervals for history output. In Abaqus/CFD the default variables are written at 20 intervals for field output.

You can turn these defaults off for an analysis in Abaqus/Standard and Abaqus/Explicit by using the odb\_output\_by\_default environment file parameter; see “Using the Abaqus environment settings,” Section 3.3.1, for details. Furthermore, specifying new output database requests in a step (see “Specifying new output requests”) overrides the default field and history output requests for that step. For large models the default output to the output database may increase the solution time and required disk space considerably. In such cases you are encouraged to review carefully the relevance of the default output variables for the proposed analysis. A C++ program is available that creates a smaller copy of a large output database by copying data from only selected frames; for more information, see “Decreasing the amount of data in an output database by retaining data at specific frames,” Section 10.15.4 of the Abaqus Scripting User’s Guide.

The odb\_output\_by\_default environment file parameter is ignored in a restart analysis. If no output requests are defined in a restart analysis, the output requests are those that propagate from the original analysis.

# Abaqus/Explicit output as a result of analysis termination

When an Abaqus/Explicit analysis encounters a fatal error in an increment, the preselected variables applicable to the current procedure are written automatically to the output database as field data. The analysis will go through an additional increment with a zero time increment size before writing these data.

# Element output

You can request that element variables (stresses, strains, section forces, element energies, etc.) be written to the output database. The output request can be repeated as often as necessary to define output for different types of element variables, different element sets, etc. The same element (or element set) can appear in several output requests. Element output to the output database is not supported for user elements.

<!-- source-page: 667 -->

# Selecting the element output variables

The following types of element variables are recognized for the purpose of defining output:

• “Element integration point” variables are associated with the integration points at which material calculations are performed (for example, components of stress and strain).   
• “Element section point” variables are associated with the cross-section of a beam, pipe, or a shell (for example, bending moments and membrane forces on the section); these variables are not available in Abaqus/CFD.   
• “Element face” variables are associated with the faces of a shell or a solid (for example, uniformly distributed pressure load on the face).   
• “Whole element” variables are attributes of an entire element (for example, the total energy content of the element).   
• “Whole element set” variables are attributes of an entire element set (for example, the current coordinates of the center of mass); these variables are available in Abaqus/Standard and Abaqus/Explicit.

The element variables that can be written to the output database are defined in “Abaqus/Standard output variable identifiers,” Section 4.2.1, “Abaqus/Explicit output variable identifiers,” Section 4.2.2, and “Abaqus/CFD output variable identifiers,” Section 4.2.3.

Input File Usage: \*ELEMENT OUTPUT list of output variables

Abaqus/CAE Usage: Step module: field or history output request editor: Select from list below

# Selecting elements for which output is required

For history output you must specify the element set (or, in Abaqus/Explicit, the tracer set) for which output is being requested. For field output specifying the element set or tracer set is optional; if you do not specify an element set or tracer set, the output will be written for all the elements in the model.

Input File Usage: \*ELEMENT OUTPUT, ELSET=element\_set\_name

Abaqus/CAE Usage: Step module: field or history output request editor: Domain: Set: set\_name

Requesting field output for the exterior elements in the model in Abaqus/Standard and Abaqus/Explicit

You can select output on the element set consisting of all the exterior three-dimensional elements in the model. This element set is generated internally by Abaqus.

Input File Usage: \*ELEMENT OUTPUT, EXTERIOR

Abaqus/CAE Usage: Step module: field output request editor: Domain: Whole model; toggle on Exterior only

<!-- source-page: 668 -->

Specifying the section point in beam, pipe, shell, and layered solid elements in Abaqus/Standard and Abaqus/Explicit

For beams, pipes, shells, or layered solids output is provided at the default section points. You can specify nondefault output points.

<table><tr><td>Input File Usage:</td><td>*ELEMENT OUTPUTlist of output pointslist of output variables</td></tr></table>

<table><tr><td>Abaqus/CAE Usage:</td><td>Step module: field or history output request editor: Output at shell, beam, and layered section points: Specify: list of output points</td></tr></table>

Requesting output at all section points in beam, pipe, shell, and layered solid elements in Abaqus/Standard and Abaqus/Explicit

You can specify that output be provided for all section points in beams, pipes, shells, and layered solids.

Input File Usage: \*ELEMENT OUTPUT, ALLSECTIONPTS

Abaqus/CAE Usage: Requesting output at all section points in beam, pipe, shell, and layered solid elements is not supported in Abaqus/CAE.

Requesting output for rebars in a reinforced model in Abaqus/Standard and Abaqus/Explicit

You can request output for rebars (“Defining reinforcement,” Section 2.2.3). If you do not explicitly request rebar output in a model with rebars, the element output requests govern the output for the matrix material only (except for section forces, where the forces in the rebar are included in the force calculation). You can request output for a particular rebar. If you do not specify the name of a rebar, output will be given for all rebars in the specified element set (or in the whole model, if you have not specified an element set).

Rebar output is available only in membrane, shell, or surface elements at the integration points and at the centroid of the element.

Input File Usage: Use the following options:

<table><tr><td>*OUTPUT, FIELD</td></tr><tr><td>*ELEMENT OUTPUT, REBAR=rebar_name, ELSET=element_set_name</td></tr><tr><td>*OUTPUT, HISTORY</td></tr><tr><td>*ELEMENT OUTPUT, REBAR=rebar_name, ELSET=element_set_name</td></tr></table>

Abaqus/CAE Usage: Use the following option to request output for rebar in addition to output for the matrix material:

Step module: field or history output request editor: Output for rebar: Include Use the following option to request output only for rebar:

Step module: field or history output request editor: Output for rebar: Only

You cannot request output for a particular rebar in Abaqus/CAE; if you request rebar output, it is given for all rebars in the specified output domain.

<!-- source-page: 669 -->

# Selecting the position of element integration point and section point output

Integration point variables and section variables in Abaqus/Standard can be written as field output to the output database in four different positions: the integration points, the centroid, averaged at nodes, or extrapolated to the nodes. Integration point variables and section variables in Abaqus/Explicit can be written as field output to the output database in three different positions: the integration points, the centroid, or the nodes. By default, output is provided at the integration points.

In most cases Abaqus/Explicit writes only integration point data to the output database. Transferring of results from the integration points to the user-specified position in Abaqus/Explicit is done by the postprocessing calculator. See “The postprocessing calculator,” Section 4.3.1, for details.

Element history output to the output database is always provided at the integration points.

Obtaining output at the integration points in Abaqus/Standard and Abaqus/Explicit

By default, the variables are output at the integration points where they are calculated. In Abaqus/Standard you can obtain the position of the integration points by using output variable COORD (see “Abaqus/Standard output variable identifiers,” Section 4.2.1).

Input File Usage: \*ELEMENT OUTPUT, POSITION=INTEGRATION POINTS

Abaqus/CAE Usage: You cannot select the position of element output in Abaqus/CAE; it is always given at the integration points.

Obtaining output at the centroid of each element in Abaqus/Standard and Abaqus/Explicit

You can choose to output the variables at the centroid of each element (the midpoint between the end nodes of a beam or a pipe element). Centroidal values are obtained by interpolation of the integration point values if the integration scheme for the element does not include a centroidal integration point. Element output of the element centroidal values is not available for recovering results within substructures; for more information, see “Using substructures,” Section 10.1.1.

Input File Usage: \*ELEMENT OUTPUT, POSITION=CENTROIDAL

Abaqus/CAE Usage: You cannot select the position of element output in Abaqus/CAE; it is always given at the integration points.

Obtaining element output extrapolated to the nodes in Abaqus/Standard and Abaqus/Explicit

You can choose to extrapolate the element integration point variables to the nodes of each element independently, without averaging the results from adjoining elements. Element output at the element nodes is not available for recovering results within substructures; for more information, see “Using substructures,” Section 10.1.1.

Input File Usage: \*ELEMENT OUTPUT, POSITION=NODES

Abaqus/CAE Usage: You cannot select the position of element output in Abaqus/CAE; it is always given at the integration points.

<!-- source-page: 670 -->

# Obtaining element output averaged at the nodes in Abaqus/Standard

You can choose to extrapolate the variables to the nodes and to then average them over all of the elements in the set that contribute to each node. For derived variables, such as stress invariants, Abaqus/Standard first averages the extrapolated tensor components over all of the elements connected to the node to obtain unique components at each node and then calculates the derived value based on the averaged components.

By default, Abaqus/Standard partitions the elements in the model into averaging regions. The partitioning is based upon the structure of the elements: element type, number of section points, type of material, single layer or composite, etc. Partitioning is not based upon the values of element properties (such as thickness), material orientations, or material constants. Averaging occurs only over elements that contribute to a node and belong to the same averaging region.

In some situations you may want the averaging regions to take into account the values of element properties. For example, since variables may be discontinuous between elements with different material constants, you may not want elements with different property definitions included in the same averaging region. In such cases you can force Abaqus/Standard to take into account values of element properties by setting the Abaqus environment parameter average\_by\_section to ON. However, in problems with many section and/or material definitions the default value of OFF will, in general, give much better performance than the nondefault value of ON.

Element output averaged at the nodes is not supported by the Visualization module of Abaqus/CAE (Abaqus/Viewer). The results are available through Abaqus Scripting Interface commands.

Input File Usage: \*ELEMENT OUTPUT, POSITION=AVERAGED AT NODES

Abaqus/CAE Usage: You cannot select the position of element output in Abaqus/CAE; it is always given at the integration points.

# Extrapolation and interpolation of element output variables in Abaqus/Standard and Abaqus/Explicit

The shape functions of the element are used for purposes of extrapolation and interpolation of output variables. Extrapolated values are generally not as accurate as the values calculated at the integration points in the areas of high stress gradients, particularly in the case of modified triangles and tetrahedra. Therefore, adequately detailed meshing is necessary around nodes where accurate nodal values of such element results are needed. If a cylindrical or spherical coordinate system is defined for the element (see “Orientations,” Section 2.2.5), the orientation at each integration point may be different. When the values at the integration points are extrapolated to the nodes, the difference in the orientation is not taken into account; therefore, if the orientation varies significantly over the elements connected to a node, the extrapolated values are not very accurate. If the material orientation undergoes significant spatial variation in a region of the model where the material behavior is truly anisotropic, a finer mesh is required to obtain accurate results even at the integration points. In that situation once the overall solution has converged with respect to the mesh density, the interpolation or extrapolation away from the integration points can also be assumed to be reasonably accurate. You should also be particularly careful when interpreting output variables extrapolated to the nodes for second-order elements with midside nodes outside the quarter-point region, such as when one edge is collapsed in two dimensions or one face is collapsed in three dimensions.
