<!-- source-page: 621 -->

# 4.1.2 OUTPUT TO THE DATA AND RESULTS FILES

Products: Abaqus/Standard Abaqus/Explicit

# References

• “Output,” Section 4.1.1   
• \*CONTACT FILE   
• \*CONTACT PRINT   
• \*EL FILE   
• \*EL PRINT   
• \*ENERGY FILE   
• \*ENERGY PRINT   
• \*FILE OUTPUT   
• \*MODAL FILE   
• \*MODAL PRINT   
• \*NODE FILE   
• \*NODE PRINT   
• \*RADIATION FILE   
• \*RADIATION PRINT   
• \*SECTION PRINT   
• \*SECTION FILE

# Overview

Output variables are available for:

• element integration points, element section points, whole elements, and element sets;   
• nodes;   
• the whole model;   
• modes in mode-based dynamics procedures;   
• surfaces in Abaqus/Standard; and   
• sections in Abaqus/Standard.

All of the output variables are defined in “Abaqus/Standard output variable identifiers,” Section 4.2.1, and “Abaqus/Explicit output variable identifiers,” Section 4.2.2. Output quantities from the elements, nodes, and whole model can be written to the data and results files in Abaqus/Standard and to the selected results file in Abaqus/Explicit. In Abaqus/Standard output quantities from eigenmodes, surfaces, and sections can also be written to the data and results files.

<!-- source-page: 622 -->

For Abaqus models defined in terms of an assembly of part instances (see “Defining an assembly,” Section 2.10.1), output in the data and results files is given in terms of node, element, set, and surface labels generated internally by Abaqus. See “Output,” Section 4.1.1, for details on how to relate the internally generated numbers and names to those you specified.

# Requesting output to the data and results files

The following sections discuss the input file syntax for requesting output to the data and results files. Abaqus/CAE automatically requests that a data file containing the default printed output for the current analysis procedure at the end of each step be generated; you cannot control the contents of the data file from within Abaqus/CAE. An analysis from Abaqus/CAE does not create a results file.

# Output to the Abaqus/Standard data file

Abaqus/Standard analysis results can be written to the data (.dat) file. Element output, nodal output, contact surface output, energy output, modal output, and section output are available.

Input File Usage: Use any of the following options to request output to the Abaqus/Standard data file:

\*CONTACT PRINT   
\*EL PRINT   
\*ENERGY PRINT   
\*MODAL PRINT   
\*NODE PRINT   
\*SECTION PRINT

These options are discussed in detail below.

# Output to the Abaqus/Standard results file

Abaqus/Standard analysis results can be written to the results (.fil) file. Element output, nodal output, contact surface output, energy output, modal output, and section output are available.

Input File Usage: Use any of the following options to request output to the Abaqus/Standard results file:

\*CONTACT FILE   
\*EL FILE   
\*ENERGY FILE   
\*MODAL FILE   
\*NODE FILE   
\*SECTION FILE

These options are discussed in detail below.

# Output to the Abaqus/Explicit results file

You can write Abaqus/Explicit analysis results to the selected results (.sel) file by specifying a results file output request in conjunction with element output, nodal output, and/or energy output requests, as

<!-- source-page: 623 -->

explained below. A results file output request can appear only once per step but remains in effect in subsequent steps unless it is redefined.

You can convert the selected results file (job-name.sel) into the results (job-name.fil) file using the convert utility described in “Obtaining results file output in Abaqus/Explicit” in “Output,” Section 4.1.1, and “Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD execution,” Section 3.2.2.

Input File Usage: Use the first option in conjunction with one or more of the subsequent options to request output to the Abaqus/Explicit selected results file:

\*FILE OUTPUT

\*EL FILE

\*ENERGY FILE

\*NODE FILE

# Output frequency

You can control the frequency of all Abaqus/Explicit results file output for a particular step by specifying the number of intervals during the step at which file output will be written, n. The data are always written at the start and end of each step in which a results file output request is active. The times at which the results are written are referred to as time marks.

If the specified number of intervals is 10, Abaqus/Explicit will write results 11 times: the values at the beginning of the step and at the end of 10 equal time intervals throughout the step. The specified number of intervals must be a positive integer.

By default, results will be written at the increment ending immediately after each time mark. Alternatively, you can choose to have the time increment size adjusted so that an increment will end exactly at each of the time marks calculated by dividing the step into n equal intervals.

Input File Usage: Use the following option to request results at the increments ending immediately after each time interval:

\*FILE OUTPUT, NUMBER INTERVAL=n, TIME MARKS=NO

Use the following option to request results at the exact time intervals:

\*FILE OUTPUT, NUMBER INTERVAL=n, TIME MARKS=YES

# Requesting output in multiple steps

Output requests apply to the step in which they are defined and to all subsequent steps until they are respecified.

One exception occurs when the step type changes from general to linear perturbation (available only in Abaqus/Standard). Output requests defined in general steps apply only to subsequent general steps; output requests defined in linear perturbation steps apply only to subsequent consecutive linear perturbation steps. In other words, output defined in a general step is independent of output defined in a linear perturbation step. Propagation between linear perturbation steps occurs only for consecutive linear perturbation steps. If a general analysis step occurs between perturbation steps, output defined in the first perturbation step will not propagate to the next perturbation step. In addition, section output requests are not propagated among linear perturbation steps in Abaqus/Standard.

<!-- source-page: 624 -->

# Element output

You can output element variables (stresses, strains, section forces, element energies, etc.) for a particular step to the Abaqus/Standard data (.dat) file, the Abaqus/Standard results (.fil) file, or the Abaqus/Explicit selected results (.sel) file. The output requests can be repeated as often as necessary within a step 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.

In general, element output requests remain in effect for subsequent steps unless they are redefined; the appearance of a single element output request in a step removes all element output requests from a previous step. See “Output,” Section 4.1.1, for a discussion of requesting output in multiple general analysis steps or linear perturbation steps.

In Abaqus/Explicit the element output is written to the selected results (.sel) file, which must be converted to the results (.fil) file as explained above.

Input File Usage: Use the following option to output element variables to the Abaqus/Standard data file:

\*EL PRINT

Use the following option to output element variables to the Abaqus/Standard results file or the Abaqus/Explicit selected results file:

\*EL FILE

# 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 the material calculations are performed (for example, components of stress and strain). For beams and pipes defined in Abaqus/Standard with a general beam section, integration point variables are available only if the output section points were specified for the section (see “Using a general beam section to define the section behavior,” Section 29.3.7). For first-order heat transfer elements the integration points are located at the corners of the element in heat capacitance calculations.   
• “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).   
• “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 only in Abaqus/Standard.

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

Abaqus/Standard allows only complete sets of basic variables (for example, all of the stress or strain components) to be written to the results file. Individual variables (such as a particular stress component) cannot be selected and must be obtained by postprocessing. Abaqus/Standard element variables can be

<!-- source-page: 625 -->

written to the data and results files at the integration points, at the centroid, averaged at the nodes, or extrapolated to the nodes.

In Abaqus/Explicit the complete stress or strain tensors can be written to the selected results file, or individual scalar variables such as equivalent plastic strain can be written. Abaqus/Explicit writes element variables to the results file only at the integration points where they are calculated.

# Selecting the elements for which output is required

You can specify the element set for which output is being requested. If you do not specify an element set, the output will be printed for all elements and, in Abaqus/Explicit, for all rebars in the model. In Abaqus/Standard output requests for rebars are governed separately, as discussed below.

Input File Usage: Use either of the following options:

\*EL PRINT, ELSET=element\_set\_name

\*EL FILE, ELSET=element\_set\_name

Specifying the section point in beams, pipes, shells, and layered solid elements

For beams, pipes, shells, or layered solid elements in Abaqus/Standard output is provided at the default section points listed in Part VI, “Elements.” You can specify nondefault output points.

In Abaqus/Explicit output is always provided at all section points for beam, pipe, and shell element output requests.

Input File Usage: Use either of the following options in Abaqus/Standard:

\*EL PRINT

list of output points

\*EL FILE

list of output points

# Requesting output for rebars in a reinforced model

In Abaqus/Standard you can request output for rebars (“Defining reinforcement,” Section 2.2.3). If you do not explicitly request rebar output in an Abaqus/Standard 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).

In beam and continuum elements in Abaqus/Standard rebar output can be obtained at the integration points only. In shell, membrane, and surface elements rebar output is available at the integration points and at the element’s centroid.

In Abaqus/Explicit output for the rebars in the specified element set (or the whole model, if you have not specified an element set) is always included for element output requests.

Input File Usage: Use either of the following options in Abaqus/Standard:

\*EL PRINT, REBAR=rebar\_name

\*EL FILE, REBAR=rebar\_name

<!-- source-page: 626 -->

# Selecting the position of element integration and section point output in Abaqus/Standard

In Abaqus/Standard integration point variables and section variables can be written to the data and results files in four different positions. By default, output is provided at the integration points.

Obtaining element output at the integration points

By default, the variables are output at the integration points where they are calculated. (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: Use either of the following options:

\*EL PRINT, POSITION=INTEGRATION POINTS

\*EL FILE, POSITION=INTEGRATION POINTS

Obtaining element output at the centroid of each element

You can choose to output the variables at the centroid of each element (the centroid of the reference surface of a shell element or 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.

Input File Usage: Use either of the following options:

\*EL PRINT, POSITION=CENTROIDAL

\*EL FILE, POSITION=CENTROIDAL

Obtaining element output averaged at the nodes

You can choose to extrapolate the variables to the nodes, then average them over all of the elements in the set that contribute to each node. For derived variables, such as the principal stress, Abaqus/Standard will first average the extrapolated tensor components over all of the elements connected to the node to obtain unique components at each node, then calculate 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 will occur 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.

<!-- source-page: 627 -->

Input File Usage: Use either of the following options:

\*EL PRINT, POSITION=AVERAGED AT NODES

\*EL FILE, POSITION=AVERAGED AT NODES

Obtaining element output extrapolated to the nodes

You can choose to extrapolate the element integration point variables to the nodes of each element independently, without averaging the results from adjoining elements.

Input File Usage: Use either of the following options:

\*EL PRINT, POSITION=NODES

\*EL FILE, POSITION=NODES

# Extrapolation and interpolation of element output variables

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 will not be 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. Element output for second-order elements with one collapsed side in two dimensions or one collapsed face in three dimensions should not be extrapolated to the nodes.

In a coupled temperature-displacement and a coupled thermal-electrical-structural analysis nodal temperatures (variable NT11) are more accurate than temperatures at the integration point (variable TEMP) extrapolated to the nodes.

For derived variables, such as the Mises equivalent stress, the components are first extrapolated or interpolated, then the derived value is calculated from the extrapolated or interpolated components. However, in linear mode-based dynamic analysis procedures where values are obtained as nonlinear combinations of modal response magnitudes (“Random response analysis,” Section 6.3.11, and “Response spectrum analysis,” Section 6.3.10), the nonlinear combinations are first calculated at the integration points. These derived values are extrapolated to the nodes or interpolated to the centroid.

# Requesting summaries in the Abaqus/Standard data file

By default in Abaqus/Standard, summaries of element variables are printed in the data file. A summary of the maximum and minimum values is printed at the end of each column in an output table. The locations of the maximum and minimum values are also printed. You can choose to suppress this summary.

Input File Usage: \*EL PRINT, SUMMARY=YES or NO

<!-- source-page: 628 -->

# Requesting totals in the Abaqus/Standard data file

In Abaqus/Standard you can print the sum (total) of each column in an output table to the data file. Totals can be used, for example, to obtain a sum of all the energies in a set of elements. By default, these totals are suppressed.

Input File Usage: \*EL PRINT, TOTALS=YES or NO

# Controlling the frequency of output

In Abaqus/Standard you can control the frequency of element output by specifying the output frequency in increments. Unless a frequency of zero is specified to suppress output, the variables will always be output at the last increment of the step.

In Abaqus/Explicit the frequency of element output is controlled as described in “Output frequency” above.

Input File Usage: Use either of the following options in Abaqus/Standard:

\*EL PRINT, FREQUENCY=n

\*EL FILE, FREQUENCY=n

# Specifying the directions for element output

For components of stress, strain, and similar material variables, 1, 2, and 3 refer to the directions in an orthogonal coordinate system. If a local orientation is not defined for the element, the stress/strain components are in the default directions defined by the convention given in “Conventions,” Section 1.2.2: global directions for solid elements; surface directions for shell, membrane, and gasket elements; and axial and transverse directions for beam and pipe elements.

If a local orientation is associated with the element, the element output variable components are in the local directions defined by the orientation (see “Orientations,” Section 2.2.5). In Abaqus/Standard you can request that the local directions be written to the results file if component output is requested for any variable (see “Output of local directions to the results file” below). In Abaqus/Explicit the local directions will always be written to the results file when tensor output is requested for any element variable. The local directions are written automatically to the output database file from both Abaqus/Standard and Abaqus/Explicit.

In large-displacement problems the local directions defined in the reference configuration are rotated into the current configuration by the average material rotation. See “State storage,” Section 1.5.4 of the Abaqus Theory Guide, for details.

# Controlling the output during eigenvalue extraction

You can control element output during natural frequency extraction (“Natural frequency extraction,” Section 6.3.5), complex eigenvalue extraction (“Complex eigenvalue extraction,” Section 6.3.6), and eigenvalue buckling analysis (“Eigenvalue buckling prediction,” Section 6.2.3) by specifying the first and last mode numbers for which output is required. By default, the first mode number is 1 and the last mode number is N, where N is the number of modes extracted. If you specify the first mode number, the default value for the last mode number is M, where M is the value specified for the first mode number.

<!-- source-page: 629 -->

Input File Usage: Use either of the following options:

\*EL PRINT, MODE=m, LAST MODE=n

\*EL FILE, MODE=m, LAST MODE=n

# Abaqus/Standard data file format

In Abaqus/Standard the printed output of variables is arranged in tables in the data file. For element variables, each row of a table corresponds to a particular location: an element, a node, a section point within an element, or an integration point. The rows that will appear in a particular table are defined by choosing an element set and, possibly, locations within each element in the set.

Each table is defined by a data line of the element output request, which specifies the variables to appear in that table. There is no limit to the number of tables that can be defined. The first columns of a table define the location—the element or node number, integration point number, etc. You choose which data will appear in the remaining columns; up to 9 variables (columns) can appear in a table. For example, output variables S and E cannot be requested on the same data line in a three-dimensional analysis because that would produce 12 columns of output. If all of the entries in a row are zero, the row is not printed.

Each table can contain only one type of output variable (whole element, section, or integration point); one type of element; and only one type of section definition. If an element output request to the data file includes more than one type of output variable, element, or section definition, Abaqus/Standard will split the output automatically into the necessary number of individual tables. All of the tables defined by the first data line of the output request will be printed, then all of the tables defined by the second data line, etc.

# Results file format

An element header record (the type 1 record described in “Results file output format,” Section 5.1.2) is created for each line of requests for each integration point and section point in an element. In addition to the element header record, a direction record (record type 85) can be written in Abaqus/Standard when complete stress or strain tensor output is requested (see below). In Abaqus/Explicit a direction record is always written when complete stress or strain tensor output is requested.

For Abaqus/Standard file output requests with multiple variables, it is advantageous to specify as many variables as possible on each data line of the element output request (up to 16). By keeping the number of lines of requests to a minimum, extra type 1 and type 85 records are avoided and the size of the results file may be reduced substantially. This is not an issue in Abaqus/Explicit. Element variables must be of the same “type” (element integration point variable; element section variable; whole element variable; etc.) to be entered on a single line—see “Output,” Section 4.1.1. In Abaqus/Standard if all results in a file output record are zero, the record is not written to the results file.

# Output of local directions to the results file

By default, in Abaqus/Standard the local coordinate directions are not written to the results file. If component output is requested, you can write the local coordinate directions to the results file. A direction record of type 85 will be written following the type 1 record.

<!-- source-page: 630 -->

In Abaqus/Explicit the local coordinate directions are always written to the selected results file as a direction record of type 85 when complete stress or strain tensor output is requested.

Tensor component output is given in the local coordinate system, which may be inherent to the element (as is the case in shells and membranes) or user-defined (“Orientations,” Section 2.2.5).

For shell elements a direction record is written for every material point in the section for which component output is requested, and a separate direction record is written for section forces and section strains. For geometrically nonlinear analysis in Abaqus/Standard the record contains the current, updated directions, except for small-strain shells and gasket elements, for which the original directions are given. For three-dimensional beams, direction output is written only if section output has been requested.

Direction output is not provided for trusses, two-dimensional beams, two-dimensional gasket elements, axisymmetric shells, axisymmetric membranes, axisymmetric gasket elements, or for values averaged at nodes. In addition, it is not provided for GKxxN-type gasket elements, which have no membrane or transverse shear deformation.

Input File Usage: Use the following option in Abaqus/Standard:

\*EL FILE, DIRECTIONS=YES

# Default element output

If you do not specify an element output request to the results file in a step (or in any previous step of the analysis), no element output will be written to the results file; similarly, if you do not specify an element output request to the data file (available only in Abaqus/Standard) in a step (or in any previous step of the analysis), no element output will be written to the data file.

# Node output

You can output nodal variables (displacements, reaction forces, etc.) for a particular step to the Abaqus/Standard data (.dat) file, the Abaqus/Standard results (.fil) file, or the Abaqus/Explicit selected results (.sel) file. The output requests can be repeated as often as necessary within a step to define output for different node sets. The same node (or node set) can appear in several output requests.

In general, nodal output requests remain in effect for subsequent steps unless they are redefined; the appearance of a single nodal output request in a step removes all nodal output requests from a previous step. See “Output,” Section 4.1.1, for a discussion of requesting output in multiple general analysis steps or linear perturbation steps.

In Abaqus/Explicit the nodal output is written to the selected results (.sel) file, which must be converted to the results (.fil) file as explained above.

Input File Usage: Use the following option to output nodal variables to the Abaqus/Standard data file:

\*NODE PRINT

Use the following option to output nodal variables to the Abaqus/Standard results file or the Abaqus/Explicit selected results file:

\*NODE FILE