4.1.3 Output to the output database

Products: ABAQUS/Standard  ABAQUS/Explicit  ABAQUS/CAE  

References

Overview

Output variables are available for:

  • element integration points, element section points, whole elements, and element sets;

  • surfaces in ABAQUS/Explicit;

  • integrated output sections in ABAQUS/Explicit;

  • nodes; and

  • the whole model.

All 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.

Model information and analysis results are stored in terms of an assembly of part instances (see Defining an assembly, Section 2.9.1).

See the ABAQUS Scripting User's Manual for a description of how to use the ABAQUS Scripting Interface or C++ to access an output database.

Requesting output to the output database

Three types of information are stored in the output database: “field” output, “history” output, and diagnostic information. Field output and history output are controlled by output database requests as described in this section. A subset of the diagnostic information that is written to the ABAQUS/Standard message file is included in the output database.

  • Field output is intended for infrequent requests for a large portion of the model and can be used to generate contour plots, animations, symbol plots, X–Y plots, and displaced shape plots in ABAQUS/CAE. Only complete sets of basic variables (for example, all the stress or strain components) can be requested as field output.

  • History output is intended for relatively frequent output requests for small portions of the model and is displayed in X–Y data plots in ABAQUS/CAE. Individual variables (such as a particular stress component) can be requested.

  • Diagnostic information is intended to provide convergence information for use in ABAQUS/CAE.

Output database requests can be repeated as often as necessary within a step to produce both field and history output at multiple frequencies.

Requesting field output

Contact surface output, element output, nodal output, and radiation output are available as field output.

Input File Usage:           Use the first option in conjunction with one or more of the subsequent options to request field output to the output database:
*OUTPUT, FIELD
*CONTACT OUTPUT
*ELEMENT OUTPUT
*NODE OUTPUT
*RADIATION OUTPUT

These options are discussed in detail below.


ABAQUS/CAE Usage: 

Step module: field output request editor


Requesting history output

Contact surface output, element output, energy output, integrated output, time incrementation output, fastener interaction output, modal output, nodal output, and radiation output are available as history output.

Requesting large amounts of history output (more than 1000 output requests) may cause performance to degrade in ABAQUS/Standard and will cause performance to degrade in ABAQUS/Explicit. For vector- or tensor-valued output variables each component is considered to be a single request. In the case of element variables history output will be generated at each integration point. For example, requesting history output of the tensor variable S (stress) for a C3D10M element will generate 24 history output requests: (6 components) (4 integration points). When requesting history output of vector- and tensor-valued variables, it is recommended that individual components be selected where available.

Input File Usage:           Use the first option in conjunction with one or more of the subsequent options to request history output to the output database:
*OUTPUT, HISTORY
*CONTACT OUTPUT
*ELEMENT OUTPUT
*ENERGY OUTPUT
*INTEGRATED OUTPUT
*INCREMENTATION OUTPUT
*INTERACTION OUTPUT
*MODAL OUTPUT
*NODE OUTPUT
*RADIATION OUTPUT

These options are discussed in detail below.


ABAQUS/CAE Usage: 

Step module: history output request editor


Requesting diagnostic information

By default, a subset of the diagnostic information that is written to the message file for ABAQUS/Standard analyses is also written to the output database. You can use the Visualization module of ABAQUS/CAE to view this diagnostic information interactively, highlighting problematic areas on a view of the model and using them to resolve errors and warnings in the analysis. For more information, see The ABAQUS/Standard message file” in “Output, Section 4.1.1, and Chapter 23, Viewing diagnostic output,” of the ABAQUS/CAE User's Manual.

Input File Usage:           Use the following option to write diagnostic information to the output database:
*OUTPUT, DIAGNOSTICS=YES

Use the following option to exclude diagnostic information:

*OUTPUT, DIAGNOSTICS=NO

ABAQUS/CAE Usage: You cannot exclude diagnostic information from the output database from within ABAQUS/CAE. Use the following option to view the saved diagnostic information:

Visualization module: ToolsJob Diagnostics


Controlling the output frequency

The frequency of output to the output database is controlled differently in ABAQUS/Standard and ABAQUS/Explicit. Control of the output frequency in ABAQUS/Explicit depends upon whether field or history output was selected.

Controlling the output frequency in ABAQUS/Standard

In ABAQUS/Standard you can specify the output frequency in terms of increments, the number of intervals during the step, the size of regular time intervals throughout the step, or time points throughout the step.

If output is requested at exact time intervals or exact time points, ABAQUS/Standard will obtain a solution corresponding to each output request time. In this case if the frequency of output to the output database file is high, the number of increments and, consequently, the computational cost of the analysis may increase considerably.

History output in ABAQUS/Standard is buffered and is written to disk only after every 10 increments of history data output or when a step has completed. Therefore, history results may not be available immediately for postprocessing.

Specifying output frequency in increments

You can specify the output frequency in increments. The data will be written at this frequency as well as at the end of each step of the analysis. Specify an output frequency of zero to suppress output.

Input File Usage:           Use one of the following options:
*OUTPUT, FIELD, FREQUENCY=n 
*OUTPUT, HISTORY, FREQUENCY=n

ABAQUS/CAE Usage: 

Step module: field or history output request editor: Save output at Every n increments


Specifying output frequency in number of intervals

You can specify the output frequency in number of intervals, n. The specified number of intervals must be a positive integer.

By default, ABAQUS/Standard adjusts the time increment (in some cases ABAQUS/Standard might violate the minimum time increment specified) to ensure that data are written at the exact times calculated by dividing the step into n equal intervals. Alternatively, you can specify that the data be written immediately after each time mark. In this case no adjustment of the time increment is necessary.

You can specify the output frequency in number of intervals only for the procedures listed in Table 4.1.3–1. In addition, this capability is not supported for linear perturbation analyses, except for modal dynamic analysis (Transient modal dynamic analysis, Section 6.3.7).

Input File Usage:           Use one of the following options to request results at the exact time intervals:
*OUTPUT, FIELD, NUMBER INTERVAL=n, TIME MARKS=YES
*OUTPUT, HISTORY, NUMBER INTERVAL=n, TIME MARKS=YES

Use one of the following options to request results at the increments ending immediately after each time interval:

*OUTPUT, FIELD, NUMBER INTERVAL=n, TIME MARKS=NO
*OUTPUT, HISTORY, NUMBER INTERVAL=n, TIME MARKS=NO

ABAQUS/CAE Usage: Use the following option to request results at the exact time intervals:

Step module: field or history output request editor: Save output at n equally spaced intervals, At Exact times indicated by the intervals

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

Step module: field or history output request editor: Save output at n equally spaced intervals, At Approximate times indicated by the intervals


Specifying output frequency in regular time interval size

You can write the results at specified regular intervals throughout the step as well as at the end of the step.

By default, ABAQUS/Standard will adjust the time increment (in some cases ABAQUS/Standard might violate the minimum time increment specified) to ensure that data will be written at the exact times, as defined by multiples of the time interval, t. Alternatively, the data can be written immediately after each time mark. In this case no adjustment of the time increment is necessary.

Specifying output frequency in regular time intervals is supported only for selected procedures listed in Table 4.1.3–1. In addition, it is not supported for linear perturbation analyses, except for modal dynamic analysis (Transient modal dynamic analysis, Section 6.3.7).

Input File Usage:           Use one of the following options to request results at the exact time intervals:
*OUTPUT, FIELD, TIME INTERVAL=t , TIME MARKS=YES
*OUTPUT, HISTORY, TIME INTERVAL=t, TIME MARKS=YES

Use one of the following options to request results at the increments ending immediately after each time interval:

*OUTPUT, FIELD, TIME INTERVAL=t , TIME MARKS=NO
*OUTPUT, HISTORY, TIME INTERVAL=t, TIME MARKS=NO

ABAQUS/CAE Usage: Use the following option to request results at the exact time intervals:

Step module: field or history output request editor: Save output at Every t units of time, At Exact times indicated by the intervals

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

Step module: field or history output request editor: Save output at Every t units of time, At Approximate times indicated by the intervals


Specifying output frequency in time points

You can write the results at specified time points throughout the step.

By default, ABAQUS/Standard adjusts the time increment (in some cases ABAQUS/Standard might violate the minimum time increment specified) to ensure that data are written at the exact time points specified. Alternatively, you can specify that the data be written immediately after each time point. In this case no adjustment of the time increment is necessary.

You can specify the output frequency in time points only for the combinations of procedures and time incrementation methods specified in Table 4.1.3–1. In addition, this capability is not supported for linear perturbation analyses, except for modal dynamic analysis (Transient modal dynamic analysis, Section 6.3.7).

Input File Usage:           Use the first option with one of the subsequent options to request results at the exact time points:
*TIME POINTS, NAME=time points name 
*OUTPUT, FIELD, TIME POINTS=time points name, TIME MARKS=YES
*OUTPUT, HISTORY, TIME POINTS=time points name, TIME MARKS=YES

Use the first option with one of the subsequent options to request results at the increments ending immediately after each time point:

*TIME POINTS, NAME=time points name 
*OUTPUT, FIELD, TIME POINTS=time points name, TIME MARKS=NO
*OUTPUT, HISTORY, TIME POINTS=time points name, TIME MARKS=NO

ABAQUS/CAE Usage: Use the following option to request results at the exact time points:

Step module: field or history output request editor: Including specific time points, At Exact times indicated by the intervals

Use the following option to request results at the increments ending immediately after each time point:

Step module: field or history output request editor: Including specific time points, At Approximate times indicated by the intervals


Table 4.1.3–1 ABAQUS/Standard procedures that support output frequency control using number of intervals, time intervals, or time points.

ProcedureTime incrementationOutput frequency
at exact times immediately after each time mark
Static stress analysis, Section 6.2.2 (except if the Riks method is used)Automatic
Fixed
Implicit dynamic analysis using direct integration, Section 6.3.2Automatic
Fixed
Uncoupled heat transfer analysis, Section 6.5.2 (output frequency in number intervals is not supported if you specify that the analysis end when steady state is reached)Automatic
Fixed
Mass diffusion analysis, Section 6.8.1 (output frequency in number intervals is not supported if you specify that the analysis end when steady state is reached)Automatic
Fixed
Coupled pore fluid diffusion and stress analysis, Section 6.7.1 (output frequency in number intervals is not supported if you specify that the analysis end when steady state is reached)Automatic
Fixed
Fully coupled thermal-stress analysis, Section 6.5.4Automatic
Fixed
Coupled thermal-electrical analysis, Section 6.6.2 (output frequency in number intervals is not supported if you specify that the analysis end when steady state is reached)Automatic
Fixed
Steady-state transport analysis, Section 6.4.1Automatic
Fixed
Subspace-based steady-state dynamic analysis, Section 6.3.9Fixed
Quasi-static analysis, Section 6.2.5Automatic
Fixed
Transient modal dynamic analysis, Section 6.3.7Fixed

Time incrementation

If the output frequency is specified at exact times and in terms of the number of intervals, in regular time intervals, or in time points, ABAQUS/Standard adjusts the time increments to ensure that data are written at the exact time points. In some cases ABAQUS may use a time increment smaller than the minimum time increment allowed in the step in the increment directly before a time point. However, ABAQUS will not violate the minimum time increment allowed for consolidation, transient mass diffusion, transient heat transfer, transient couple thermal-electrical, and transient coupled temperature-displacement analyses. For these procedures if a time increment smaller than the minimum time increment is required, ABAQUS will use the minimum time increment allowed in the step and will write output data at the first increment after the time point.

When the output frequency is specified at exact times and in terms of the number of intervals, in regular time intervals, or in time points, the number of increments necessary to complete the analysis might increase, which might adversely affect performance.

Default output

If you do not specify the output frequency, field and history output will be written at every increment of the analysis for all procedure types except dynamic and modal dynamic analyses; output will be written every 10 increments for these procedure types.

Controlling the output frequency for field output in ABAQUS/Explicit

Field output data are always written at the start and end of each step in which the output request is active. In addition, you can specify the output frequency in terms of the number of intervals during the step, the size of regular time intervals throughout the step, or time points throughout the step. The times at which the results are written are referred to as time marks.

Specifying field output frequency in number of intervals

You can specify the output frequency in number of intervals, n. The specified number of intervals must be a positive integer. For example, if the specified number of intervals is 10, ABAQUS/Explicit will write field data 11 times: the values at the beginning of the step and at the end of 10 equal time intervals throughout the step.

By default, field data will be written at the increment ending immediately after each time mark. Alternatively, when you specify the output frequency in number of intervals, 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:
*OUTPUT, FIELD, NUMBER INTERVAL=n, TIME MARKS=NO

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

*OUTPUT, FIELD, NUMBER INTERVAL=n, TIME MARKS=YES

ABAQUS/CAE Usage: Use the following option to request results at the increments ending immediately after each time interval:

Step module: field output request editor: Save output at n equally spaced intervals, At Approximate times indicated by the intervals

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

Step module: field output request editor: Save output at n equally spaced intervals, At Exact times indicated by the intervals


Specifying field output frequency in regular time interval size

Alternatively, you can write the results at specified regular intervals throughout the step as well as at the beginning and end of the step. The time increment size will not be adjusted to meet the specified time marks; results will be written at the increment ending immediately after each time mark, as defined by multiples of the time interval, t.

Input File Usage:           
*OUTPUT, FIELD, TIME INTERVAL=t

ABAQUS/CAE Usage: 

Step module: field output request editor: Save output at Every t units of time


Specifying field output frequency in time points

You can write the results at specified time points throughout the step. Regular time intervals between time points are not required; you can specify any desired time points at which the field output is to be written.

Input File Usage:           Use the following option to request results at the exact time points:
*TIME POINTS, NAME=time points name 
*OUTPUT, FIELD, TIME POINTS=time points name, TIME MARKS=YES

Use the following option to request results at the increments ending immediately after each time point:

*TIME POINTS, NAME=time points name 
*OUTPUT, FIELD, TIME POINTS=time points name, TIME MARKS=NO

ABAQUS/CAE Usage: Use the following option to request results at the exact time points:

Step module: field output request editor: Including specific time points, At Exact times indicated by the intervals

Use the following option to request results at the increments ending immediately after each time point:

Step module: field output request editor: Including specific time points, At Approximate times indicated by the intervals


Default field output

If you do not specify the output frequency (in either number of intervals, time interval size, or time points), field output will be written at 20 equally spaced intervals throughout the step.

Controlling the output frequency for history output in ABAQUS/Explicit

If history output is selected, you can specify the output frequency in terms of either increments or regular intervals throughout the step.

Specifying history output frequency in increments

You can specify the output frequency in increments. The data will be written at this frequency as well as at the end of each step of the analysis.

Input File Usage:           
*OUTPUT, HISTORY, FREQUENCY=n

ABAQUS/CAE Usage: 

Step module: history output request editor: Save output at Every n time increments


Specifying history output frequency in regular time interval size

Alternatively, you can write the results at specified regular intervals throughout the step as well as at the end of the step. The time increment size will not be adjusted to meet the specified time marks; results will be written at the increment ending immediately after each time mark, as defined by multiples of the time interval, t.

Input File Usage:           
*OUTPUT, HISTORY, TIME INTERVAL=t

ABAQUS/CAE Usage: 

Step module: history output request editor: Save output at Every t units of time


Default history output

If you do not specify the output frequency (in either increments or time interval size), history output will be written at 200 equally spaced intervals throughout the step.

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.

The only 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.

Specifying new output requests

By default, all output requests defined in previous steps are removed when new requests are defined, regardless of the type of output request being defined. In other words, a new field output request in a step removes all field and history output requests defined in previous steps. Only output requests defined in previous steps are affected; other output requests defined in the same step are not affected.

This behavior is the same as the behavior for output requests to the ABAQUS/Standard data file (file_name.dat) and the ABAQUS/Standard and ABAQUS/Explicit results files (file_name.fil); see Output to the data and results files, Section 4.1.2.

Because all existing output requests are removed when a new request is defined in a step, all output requests within the same step are treated as new (i.e., additional output requests or replacement output requests are treated as equivalent to new output requests).

Alternatively, you can specify a new output request without removing all previously defined output requests.

Input File Usage:           Use one of the following options to remove all existing output requests and to specify new requests:
*OUTPUT, FIELD, OP=NEW
*OUTPUT, HISTORY, OP=NEW

Use one of the following options to specify additional output requests without removing all existing output requests:

*OUTPUT, FIELD, OP=ADD
*OUTPUT, HISTORY, OP=ADD

ABAQUS/CAE Usage: 

Step module: Create Field Output Request or Create History Output Request


ABAQUS/CAE automatically respecifies all previously defined output requests when you create a new request.

Replacing or removing an output request

You can replace an output request of the same type (e.g., field or history) and frequency with a new request. No other previously defined requests will be affected.

You cannot replace an output request to change its frequency. If no matching request is found, the request specified is simply added to the step.

To remove a previously defined request, you can replace the output request without specifying any new output requests.

Input File Usage:           Use one of the following options to replace an output request with a new request:
*OUTPUT, FIELD, OP=REPLACE
*OUTPUT, HISTORY, OP=REPLACE

ABAQUS/CAE Usage: 

Step module: Field Output Requests Manager or History Output Requests Manager: Edit or Delete


Suppressing output requests defined in previous steps

To suppress completely all output requests that have been defined in previous steps, you can specify an output frequency of 0.

Preselected output requests

There are two ways to define output variable requests quickly and easily. Both methods are available for field and history output requests and for the individual output requests used for requesting specific variable types (e.g., nodal). The use of these methods with individual output requests for specific variable types is explained in detail later in this section.

Requesting procedure-specific preselected output requests

You can activate a procedure-specific set of commonly requested output variables. See Table 4.1.3–2 for a list of procedure types and their accompanying preselected variables. The variables written to the output database may change if the procedure type changes between steps.

If you request preselected field or history output and request additional output variables using individual output requests for specific variable types, the variables requested will be appended to the variables contained in the preselected list.

For geometrically nonlinear analysis in ABAQUS/Standard, E is not available for output and LE is output by default. For linear perturbation analyses and geometrically linear analyses in ABAQUS/Standard, LE and NE strain output requests yield the same output as E. For geometrically linear analysis in ABAQUS/Explicit, LE is output.

ABAQUS may omit some preselected variables from the analysis results. ABAQUS omits preselected output variables if they are not applicable for the element type used to mesh the model or if other factors make the variables unsuitable for the analysis.

Input File Usage:           Use one of the following options:
*OUTPUT, FIELD, VARIABLE=PRESELECT
*OUTPUT, HISTORY, VARIABLE=PRESELECT

ABAQUS/CAE Usage: 

Step module: field or history output request editor: Preselected defaults


Table 4.1.3–2 List of preselected variables for various procedure types.

Procedure typePreselected element variables (field)Preselected nodal and surface variables (field)Preselected energy variables (history)
Annealingnonenonenone
Complex frequency extraction Unone
Coupled pore fluid diffusion/stressS, E, VOIDR, SAT, PORU, RF, CF, PFL, PFLA, PTL, PTLA, TPFL, TPTLALLAE, ALLCD, ALLFD, ALLIE, ALLKE, ALLPD, ALLSE, ALLVD, ALLDMD, ALLWK, ALLKL, ALLQB, ALLEE, ALLJD, ALLSD, ETOTAL
Coupled thermal-electricHFL, EPGNT, RFL, EPOTALLAE, ALLCD, ALLFD, ALLIE, ALLKE, ALLPD, ALLSE, ALLVD, ALLDMD, ALLWK, ALLKL, ALLQB, ALLEE, ALLJD, ALLSD, ETOTAL
Direct cyclicS, E, PE, PEEQ, PEMAGU, RF, CFALLAE, ALLCD, ALLFD, ALLIE, ALLKE, ALLPD, ALLSE, ALLVD, ALLDMD, ALLWK, ALLKL, ALLQB, ALLEE, ALLJD, ALLSD, ETOTAL
Direct-integration implicit dynamic (with an output frequency of 10)S, E, PE, PEEQ, PEMAGU, V, A, RF, CF, CSTRESS, CDISPALLAE, ALLCD, ALLFD, ALLIE, ALLKE, ALLPD, ALLSE, ALLVD, ALLDMD, ALLWK, ALLKL, ALLQB, ALLEE, ALLJD, ALLSD, ETOTAL
Direct-solution steady-state dynamicS, EU, V, A, RF, CFALLKE, ALLSE, ALLVD, ALLWK
Eigenfrequency extraction Unone
Eigenvalue buckling prediction Unone
Explicit dynamicS, LE, PE, PEEQU, V, A, RF, CSTRESSALLKE, ALLSE, ALLWK, ALLPD, ALLCD, ALLVD, ALLDMD, ALLAE, ALLIE, ALLFD, ETOTAL
Fully coupled thermal-stress in ABAQUS/StandardS, E, PE, PEEQ, PEMAG, HFLU, RF, CF, NT, RFL, CSTRESS, CDISPALLAE, ALLCD, ALLFD, ALLIE, ALLKE, ALLPD, ALLSE, ALLVD, ALLDMD, ALLWK, ALLKL, ALLQB, ALLEE, ALLJD, ALLSD, ETOTAL
Fully coupled thermal-stress in ABAQUS/ExplicitS, LE, PE, PEEQ, HFLU, V, A, RF, CSTRESS, NT, RFLALLKE, ALLSE, ALLWK, ALLPD, ALLCD, ALLVD, ALLDMD, ALLAE, ALLIE, ALLFD, ALLIHE, ALLHF, ETOTAL
Geostatic stress fieldS, E, POR, SAT, VOIDRU, RF, CF, CSTRESS, CDISPALLAE, ALLCD, ALLFD, ALLIE, ALLKE, ALLPD, ALLSE, ALLVD, ALLDMD, ALLWK, ALLKL, ALLQB, ALLEE, ALLJD, ALLSD, ETOTAL
Heat transferHFLNT, RFLnone
Linear static perturbationS, EU, RF, CFALLAE, ALLCD, ALLFD, ALLIE, ALLKE, ALLPD, ALLSE, ALLVD, ALLDMD, ALLWK, ALLKL, ALLQB, ALLEE, ALLJD, ALLSD, ETOTAL
Mass diffusionCONC, MFLNNC, RFLnone
Modal dynamic (with an output frequency of 10)S, EU, V, A, RF, CFALLAE, ALLCD, ALLFD, ALLIE, ALLKE, ALLPD, ALLSE, ALLVD, ALLDMD, ALLWK, ALLKL, ALLQB, ALLEE, ALLJD, ALLSD, ETOTAL
Quasi-staticS, E, PE, PEEQ, PEMAG, CE, CEEQ, CEMAGU, RF, CF, CSTRESS, CDISPALLAE, ALLCD, ALLFD, ALLIE, ALLKE, ALLPD, ALLSE, ALLVD, ALLDMD, ALLWK, ALLKL, ALLQB, ALLEE, ALLJD, ALLSD, ETOTAL
Random responseS, EU, V, Anone
Response spectrumS, EU, RF, CFALLKE, ALLSE, ALLWK
StaticS, E, PE, PEEQ, PEMAGU, RF, CF, CSTRESS, CDISPALLAE, ALLCD, ALLFD, ALLIE, ALLKE, ALLPD, ALLSE, ALLVD, ALLDMD, ALLWK, ALLKL, ALLQB, ALLEE, ALLJD, ALLSD, ETOTAL
Steady-state dynamicS, EU, V, A, RF, CFALLKE, ALLSE, ALLWK
Steady-state transportS, EU, RF, CF, CSTRESS, CDISPALLAE, ALLCD, ALLFD, ALLIE, ALLKE, ALLPD, ALLSE, ALLVD, ALLDMD, ALLWK, ALLKL, ALLQB, ALLEE, ALLJD, ALLSD, ETOTAL
Subspace-based steady-state dynamicS, EU, V, A, RF, CFALLKE, ALLSE, ALLVD, ALLWK

Requesting all variables applicable to the current procedure and material type

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.

Input File Usage:           Use one of the following options:
*OUTPUT, FIELD, VARIABLE=ALL
*OUTPUT, HISTORY, VARIABLE=ALL

ABAQUS/CAE Usage: 

Step module: field or history output request editor: All


Default output

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.

You can turn these defaults off for an analysis 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 9.15.4 of the ABAQUS Scripting User's Manual.

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.

Selecting eigenmodes desired for output in ABAQUS/Standard

In an eigenvalue extraction or eigenvalue buckling analysis, you can select the eigenmodes for which the output requests are desired. If you do not specify a list of eigenmodes, output is produced for all of the extracted eigenmodes. To suppress all output for an analysis, specify an output frequency of zero.

Input File Usage:           
*OUTPUT, FIELD, MODE LIST

ABAQUS/CAE Usage: 

Step module: field output request editor: Save output at Specify list of eigenmodes


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.

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 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 output database are defined in ABAQUS/Standard output variable identifiers, Section 4.2.1, and ABAQUS/Explicit output variable identifiers, Section 4.2.2.

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 name: set_name


Specifying the section point in beam, shell, and layered solid elements

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

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

ABAQUS/CAE Usage: 

Step module: field or history output request editor: Output at shell, beam, and layered section points: Specify: list of output points


Requesting output for rebars in a reinforced model

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:
*OUTPUT, FIELD
*ELEMENT OUTPUT, REBAR=rebar_name, ELSET=element_set_name
*OUTPUT, HISTORY
*ELEMENT OUTPUT, REBAR=rebar_name, ELSET=element_set_name

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.


Selecting the position of element integration point and section point output

Integration point variables and section variables 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. ABAQUS writes only integration point data to the output database. Transferring of results from the integration points to the user-specified position 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

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

You can choose to output the variables at the centroid of each element (the midpoint between the end nodes of a beam element). Centroidal values are obtained through the postprocessing calculator by interpolation of the integration point values if the integration scheme for the element does not include a centroidal integration point.

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

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:           
*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.

Extrapolation and interpolation of element output variables

The shape functions of the element are used by the postprocessing calculator 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.

For derived variables, such as Mises equivalent stress, the components are first extrapolated or interpolated. The derived value is then calculated from the extrapolated or interpolated components. However, in linear mode-based dynamic analysis procedures where derived 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 then extrapolated to the nodes or interpolated to the centroid.

Controlling the output frequency

The frequency of element output is controlled as described above in “Controlling the output frequency.”

Requesting preselected output

You can request the preselected, procedure-specific element output variables described in Table 4.1.3–2. In this case you can specify additional variables as part of the output request.

Alternatively, you can request all element variables applicable to the current procedure and material type. In this case any additional variables you specify are ignored.

Input File Usage:           Use the following option to request the preselected element output variables:
*ELEMENT OUTPUT, VARIABLE=PRESELECT

Use the following option to request all applicable element output variables:

*ELEMENT OUTPUT, VARIABLE=ALL

ABAQUS/CAE Usage: 

Step module: field or history output request editor: Preselected defaults or All


Specifying the directions for element output

For components of stress, strain, and similar material variables 1, 2, and 3 refer to the directions for 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 Orientations, Section 2.2.5: global directions for solid elements, surface directions for shell and membrane elements, and axial and transverse directions for beam elements.

By default, the element material directions for element field output are written to the output database. If a local orientation is associated with the element, by default the results displayed in ABAQUS/CAE are in the directions defined by the local orientation. These directions can be visualized in ABAQUS/CAE by selecting PlotMaterial Orientations in the Visualization module. You can choose to suppress the direction output to the output database.

Input File Usage:           Use the following option to indicate that the element material directions should not be written to the output database:
*ELEMENT OUTPUT, FIELD, DIRECTIONS=NO

ABAQUS/CAE Usage: 

Step module: field output request editor: toggle off Include local coordinate directions when available


Node output

You can output nodal variables (displacements, reaction forces, etc.) to the output database. The output request can be repeated as often as necessary to define output for different node sets. The same node (or node set) can appear in several output requests.

Selecting the nodal output variables

The nodal variables that can be written to the output database are defined in the “Nodal variables” section of ABAQUS/Standard output variable identifiers, Section 4.2.1, and ABAQUS/Explicit output variable identifiers, Section 4.2.2.

Input File Usage:           
*NODE OUTPUT
list of output variables

ABAQUS/CAE Usage: 

Step module: field or history output request editor: Select from list below


Selecting the nodes for which output is required

For history output you must specify the node set (or, in ABAQUS/Explicit, the tracer set) for which output is being requested. For field output the specification of the node set or tracer set is optional; if you do not specify a node set or tracer set, the output will be written for all the nodes in the model.

Input File Usage:           
*NODE OUTPUT, NSET=node_set_name

ABAQUS/CAE Usage: 

Step module: field or history output request editor: Domain: Set name: set_name


Controlling the output frequency

The frequency of nodal output is controlled as described above in “Controlling the output frequency.”

Controlling the precision

You can control the precision of nodal output for an analysis.

Input File Usage:           Use the following command line option to request single-precision nodal output:

abaqus job=job-name output_precision=single

Use the following command line option to request double-precision nodal output:

abaqus job=job-name output_precision=full


ABAQUS/CAE Usage: 

Job module: job editor: Precision: Nodal output precision: Single or Full


Requesting preselected output

You can request the preselected, procedure-specific nodal output variables described in Table 4.1.3–2. In this case you can specify additional variables as part of the output request.

Alternatively, you can request all nodal variables applicable to the current procedure type. In this case any additional variables you specify are ignored.

Input File Usage:           Use the following option to request the preselected nodal output variables:
*NODE OUTPUT, VARIABLE=PRESELECT

Use the following option to request all applicable nodal output variables:

*NODE OUTPUT, VARIABLE=ALL

ABAQUS/CAE Usage: 

Step module: field or history output request editor: Preselected defaults or All


Specifying the directions for nodal output

For nodal variables 1, 2, and 3 refer to the global directions X, Y, and Z, respectively. For axisymmetric elements 1 and 2 refer to the global directions r and z. Nodal results are written to the output database in the global directions. If a local coordinate system is defined at a node (see Transformed coordinate systems, Section 2.1.5), the local nodal transformations are written to the output database as well. You can apply these transformations to the results in the Visualization module of ABAQUS/CAE to view components in the local systems.

Visualizing boundary conditions

Boundary conditions can be visualized in the Visualization module of ABAQUS/CAE by selecting ViewODB Display Options. Click the Entity Display tab in the dialog box that appears.

In an ABAQUS/Standard analysis boundary condition information is written to the output database only when some nodal output variables are requested as field output.

Tracer particle output from ABAQUS/Explicit

In ABAQUS/Explicit tracer particles can be used to obtain output at specific material points that may not correspond to a fixed location in the mesh if adaptive meshing is used. Tracer particles follow the material motion throughout an analysis regardless of the mesh motion, which makes them ideal for use with adaptive meshing (see Defining ALE adaptive mesh domains in ABAQUS/Explicit, Section 12.2.2). Both nodal and element output can be obtained at tracer particles.

Defining tracer particles

You define the initial location of each tracer particle to be coincident with a node, called the “parent node.” These parent nodes are grouped into a tracer set; you must assign a name to the tracer set when you define the tracer particles.

Input File Usage:           
*TRACER PARTICLE, TRACER SET=tracer_set_name
list of parent nodes (either node numbers or node set labels)

ABAQUS/CAE Usage: Tracer particles are not supported in ABAQUS/CAE.

Particle birth stages

Sets of tracer particles can be released from the current locations of the parent nodes at multiple times during a step. Each release of tracer particles is referred to as a “particle birth.” After particle birth the tracer particles follow the motion of the associated material regardless of the motion of the mesh. You can indicate the number of particle birth stages in a step, n. One particle birth will occur at the beginning of the step, and the rest of the stages will be evenly spaced throughout the step. If you do not specify a number of particle birth stages, a single particle birth will occur at the beginning of the step.

Input File Usage:           
*TRACER PARTICLE, TRACER SET=tracer_set_name, PARTICLE BIRTH STAGES=n

ABAQUS/CAE Usage: Tracer particles are not supported in ABAQUS/CAE.

Tracer particles in the output database

Tracer sets will appear as both node and element sets in the output database. If a tracer set has multiple birth stages, additional node and element sets will be created that group all the tracer particles associated with a given birth stage. These subsets are named by appending the birth stage number to the tracer set name. For example, if a tracer set with the name INLET is defined with two particle birth stages, three node sets and three element sets will be created in the output database: INLET Stage 1, INLET Stage 2, and INLET (which contains all the nodes/elements from both INLET Stage 1 and INLET Stage 2).

Internal field output requests are generated automatically for the requested output variables for all the elements or nodes in the domain that completely defines the space of possible tracer particle locations. This region is determined by ABAQUS/Explicit and typically corresponds to the elements attached to the parent nodes and any intersecting adaptive mesh domains. The postprocessing calculator (see The postprocessing calculator, Section 4.3.1) will compute the value of any requested output quantity at a tracer particle by interpolating the results from the element that encompasses the particle at the time of output.

Requesting output at tracer particles

You can request element or nodal output for a particular tracer set. Output will be given for all tracer particles that are associated with the specified tracer set name.

Input File Usage:           Use one of the following options:
*NODE OUTPUT, TRACER SET=tracer_set_name 
*ELEMENT OUTPUT, TRACER SET=tracer_set_name

ABAQUS/CAE Usage: Tracer particle output is not supported in ABAQUS/CAE.

Field output at tracer particles

Displacement is the only valid field request for tracer particles. You can obtain the positions of the tracer particles in a specific tracer set by requesting displacements as nodal field output. Tracer particle displacements are output automatically if displacement output is requested for the entire model. You can use the node and element sets created for tracer particles in the output database to control the display of tracer particles in the Visualization module of ABAQUS/CAE.

Input File Usage:           Use both of the following options:
*OUTPUT, FIELD
*NODE OUTPUT, TRACER SET=tracer_set_name 
U

ABAQUS/CAE Usage: Tracer particle output is not supported in ABAQUS/CAE.

History output at tracer particles

Requesting history output for tracer particles is similar to requesting history output for elements and nodes. Any valid element integration point variable can be requested. U, V, A, and COORD are the only valid nodal requests. Whole element variables and element section variables cannot be requested. History data are available for a tracer particle only after its birth.

A tracer particle history output request triggers an internal field output request for the desired variables for all the elements or nodes in the domain that completely defines the space of possible tracer particle locations.

Input File Usage:           Use the following options:
*OUTPUT, HISTORY
*NODE OUTPUT, TRACER SET=tracer_set_name 
*ELEMENT OUTPUT, TRACER SET=tracer_set_name

ABAQUS/CAE Usage: Tracer particle output is not supported in ABAQUS/CAE.

Tracer particle propagation in multiple steps

Once defined, all tracer particles remain active in subsequent steps. However, no further particle births occur in the steps that follow the tracer set definition. You can define new tracer particles in subsequent steps by specifying a new tracer set name. The same tracer set name cannot be used more than once within an analysis.

Tracer particle deactivation

Individual tracer particles are deactivated if they flow out of the mesh across an Eulerian boundary or are currently tracking material points inside a failed element that has been deleted from the mesh. History data for tracer particles are zero at all times after deactivation.

Controlling the output frequency at tracer particles

The frequency of tracer particle output is controlled as described above in “Controlling the output frequency.”

Warning:  Requesting tracer set history output at a high frequency may cause the output database (.odb) to become large. The disk space required to store the field data is directly proportional to the size of the adaptive mesh domain and the number of tracer sets. The disk space usage is independent of the number of tracer particles in a tracer set. The output database file size is reduced after the postanalysis calculation is performed.

Integrated output in ABAQUS/Explicit

An integrated output request is used to write the time history of variables such as the total force transmitted across a surface. The values are computed using the material point stresses and the hourglass-mode forces in the elements underlying the surface. Integrated output is available only as history output.

Selecting the integrated output variables

The integrated variables that can be written to the output database are defined in the “Integrated variables” section of ABAQUS/Explicit output variable identifiers, Section 4.2.2.

Input File Usage:           
*INTEGRATED OUTPUT
list of output variables

ABAQUS/CAE Usage: 

Step module: history output request editor: Select from list below


Selecting the surface over which integrated output is required

You can specify the surface directly for an integrated output request. Alternatively, you can associate an integrated output section that identifies the surface (see Integrated output section definition, Section 2.5.1) with the integrated output request.

Integrated output can be requested for a surface that includes facets, edges, or ends of various types of deformable elements. The surface can include facets of three-dimensional solid elements and continuum shell elements; edges of two-dimensional solid elements, membrane elements, conventional shell, and surface elements; and ends of beam elements and truss elements.

Specifying the surface for integrated output directly

If you specify the surface for an integrated output request directly, any vector output variables are given with respect to a fixed global coordinate system and the total moment transmitted across the surface, SOM, is computed about the fixed global origin. See Defining element-based surfaces, Section 2.3.2, for information on defining element-based surfaces.

Input File Usage:           Use both of the following options:
*SURFACE, NAME=surface_name, TYPE=ELEMENT
*INTEGRATED OUTPUT, SURFACE=surface_name

ABAQUS/CAE Usage: You cannot specify the surface for an integrated output request directly in ABAQUS/CAE; you must create an integrated output section as described below.

Specifying the surface through an integrated output section definition

If you associate an integrated output section definition with an integrated output request, the integrated output variables can be obtained in a local coordinate system that can translate and/or rotate with the deformation (see Figure 4.1.3–1). In addition, the total moment transmitted across the surface, SOM, can be computed about a moving location.

Figure 4.1.3–1 A user-defined local coordinate system.

Input File Usage:           Use both of the following options:
*INTEGRATED OUTPUT SECTION, NAME=section_name, SURFACE=surface_name
*INTEGRATED OUTPUT, SECTION=section_name

ABAQUS/CAE Usage: 

Step module:

OutputIntegrated Output SectionsCreate: Name: section_name: select regions for the surface

History output request editor: Domain: Integrated output section: section_name


Requesting integrated output for “force-flow” studies

To study the “force-flow” through various paths in a model, you must create interior surfaces that cut through one or more regions (similar to a cross-section) so that you can request integrated output of the total force transmitted across these surfaces. You can create such interior surfaces over the element facets, edges, or ends by simply cutting through one or more regions of the model with a plane; see Creating interior cross-section surfaces” in “Defining element-based surfaces, Section 2.3.2, for more information.

Input File Usage:           Use both of the following options:
*SURFACE, NAME=surface_name, TYPE=CUTTING SURFACE
*INTEGRATED OUTPUT, SURFACE=surface_name

ABAQUS/CAE Usage: You cannot specify the surface for an integrated output request directly in ABAQUS/CAE; you must create an integrated output section as described above.

Controlling the output frequency

The frequency of integrated output is controlled as described above in “Controlling the output frequency for history output in ABAQUS/Explicit.”

Requesting preselected output

You can request the preselected integrated output variables SOF and SOM. In this case you can also specify additional variables as part of the output request.

Alternatively, you can request all integrated variables applicable to the current procedure type. In this case any additional variables that you specify are ignored.

If you do not request the preselected variables or all variables, you must specify the variables individually.

Input File Usage:           Use the following option to request the preselected integrated output variables:
*INTEGRATED OUTPUT, VARIABLE=PRESELECT 
optional additional variables

Use the following option to request all integrated output variables relevant to the current procedure type:

*INTEGRATED OUTPUT, VARIABLE=ALL

Use the following option to specify individual integrated output variables:

*INTEGRATED OUTPUT
individual variables

ABAQUS/CAE Usage: 

Step module: history output request editor: Preselected defaults or All


Limitations when using integrated output requests

Integrated output requests are subject to the following limitations:

  • Integrated output can be requested over a surface that includes facets, edges, or ends of various types of deformable elements. The surface can include facets of three-dimensional solid elements and continuum shell elements; edges of two-dimensional solid elements, membrane elements, conventional shell, and surface elements; and ends of beam elements and truss elements. The surface should not contain facets of axisymmetric elements or facets of rigid elements.

  • When defining the surface, elements on only one side of the surface must be used. ABAQUS/Explicit computes the integrated output variables using the stresses and hourglass-mode forces in elements underlying the surface as in a free-body diagram.

  • The defined surface must cut completely through the mesh, form a closed surface, or be on the exterior of the body. Figure 4.1.3–2 presents some typical cases of valid surfaces. If the surface cuts only partially through the mesh, a valid free-body diagram cannot be isolated (see Figure 4.1.3–3) and incorrect answers may be computed.

    Figure 4.1.3–2 Valid section definitions.

    Figure 4.1.3–3 Invalid section definitions.

  • Elements attached to the surface can be on either side of the surface but must not cross the defined surface. Figure 4.1.3–3 presents a few invalid cases.

  • The total force and the total moment in the section are computed based only on the stresses (internal forces) in the identified elements. Thus, inaccurate results may be obtained if distributed body loads are present in these elements since their effect on the total force in the section is not included. Common examples are the inertial loading in dynamic analyses, gravity loads, distributed body forces, and centrifugal loads. In these cases the total force in the section may depend on the choice of elements used to define the section as illustrated in Figure 4.1.3–4(a).

    Figure 4.1.3–4 Total force in the section.

    Assuming that gravity loading is the only active load, the element stresses will be different in the two elements. Hence, if the same surface is defined first using element 1 and then using element 2, different answers for the total force will be obtained. In a similar way the effects of any distributed body fluxes (heat, electrical, etc.) prescribed in the identified elements are not included.

  • Depending on which side of the surface is used to define the section, different answers will be obtained in analyses similar to the case illustrated in Figure 4.1.3–4(b). Assuming a quasi-static analysis with the concentrated loads shown in the figure being the only active loads, a zero total force is reported if the surface is defined using element 1 and a nonzero force equal to the sum of the concentrated loads is obtained if the surface is defined using element 2.

Total energy output

You can output the total energy of the model or of a specific element set to the output database. Energy output is available only as history output. Energy output requests are not available for the following procedures:

Selecting the energy output variables

The energy variables that can be written to the output database are defined in the “Total energy output quantities” section of ABAQUS/Standard output variable identifiers, Section 4.2.1, and ABAQUS/Explicit output variable identifiers, Section 4.2.2.

Input File Usage:           
*ENERGY OUTPUT
list of output variables

ABAQUS/CAE Usage: 

Step module: history output request editor: Select from list below


Selecting the element set for which total energy output is required

You can specify the element set for which total energy output is being requested. In this case the energies are summed for all the elements in the specified set. You cannot specify an element set for the following procedures:

The following energies are not available as element set quantities: ALLWK, ALLFD, ALLQB, ALLKL, ALLFC, and ETOTAL.

If you do not specify an element set, the total energies for the whole model will be output. If total energy output for both the whole model and for different element sets is desired, the energy output requests must be repeated: once without a specified element set to request energy output for the whole model and once for each specified element set.

Input File Usage:           
*ENERGY OUTPUT, ELSET=element_set_name

ABAQUS/CAE Usage: 

Step module: history output request editor: Domain: Set name: set_name


Controlling the output frequency

The frequency of energy output is controlled as described above in “Controlling the output frequency.”

Requesting preselected output

You can request the preselected, procedure-specific energy output variables described in Table 4.1.3–2. In this case you can specify additional variables as part of the output request.

Alternatively, you can request all energy variables applicable to the current procedure and material type. In this case any additional variables you specify are ignored.

Input File Usage:           Use the following option to request the preselected energy output variables:
*ENERGY OUTPUT, VARIABLE=PRESELECT

Use the following option to request all applicable energy output variables:

*ENERGY OUTPUT, VARIABLE=ALL

ABAQUS/CAE Usage: 

Step module: history output request editor: Preselected defaults or All


Filtering history output in ABAQUS/Explicit

Element, nodal, contact, integrated, and fastener interaction history output can be pre-filtered before it is written to the output database.

Defining a low-pass Infinite Impulse Response filter

You can define three types of low-pass Infinite Impulse Response filters as part of the model definition. Typical magnitude curves for analog type filters are presented in Figure 4.1.3–5.

Figure 4.1.3–5 Typical magnitude curves for low-pass filters.

The Butterworth filter is very common; its response in the pass band is known as maximally flat. The Type I Chebyshev filter has a sharper transition between the pass band and the stop band, but it has a ripple in the pass band. The Type II Chebyshev filter also has a sharper transition between the pass band and the stop band than a Butterworth filter of the same order, but it has a ripple in the stop band. The higher the order of the filter, the narrower the transition band. However, the computational cost increases as the order increases. In addition, for high-order filters the phase lag, which is the time delay between the filtered and unfiltered signal, may become significant. For most applications filter orders of two or four are sufficiently accurate.

To define a Butterworth filter, you must specify the cutoff frequency, , and the filter order, N. Since the implementation of the filters is done using cascades of second-order sections, ABAQUS expects an even number for the filter order. If you specify an odd number for the order, the order will be changed internally to the closest greater even number. The default value for the order is two, and the highest order that can be prescribed is twenty. For the Chebyshev filters you must also specify an additional parameter, the ripple factor. The ripple factor is equal to for a Type I Chebyshev filter and is equal to for a Type II Chebyshev filter (see Figure 4.1.3–5).

No checks are performed to ensure that the cutoff frequency is appropriate; for example, ABAQUS does not check that only the noise of the signal is eliminated. You need to know the range of the physical frequencies that are expected in the solution, and you must prescribe a cutoff frequency greater than these frequencies. In addition, the cutoff frequency should be less than half the sampling frequency (the sampling frequency is the inverse of the time increment); otherwise, no filtering is performed. The values of variables at time zero (zero increment) are used as the initial conditions (or start-up conditions). The filtered history output variables are continuous over the steps; i.e., the start-up conditions are used only in the first step.

You must assign each filter definition a name that can be used to refer to the filter from an output request.

Input File Usage:           Use one of the following options:
*FILTER, NAME=filter_name, TYPE=BUTTERWORTH 
*FILTER, NAME=filter_name, TYPE=CHEBYS1
*FILTER, NAME=filter_name, TYPE=CHEBYS2

ABAQUS/CAE Usage: 

Step module: ToolsFilterCreate: Name: filter_name; Butterworth, Chebyshev 1, or Chebyshev 2


Filtering using the low-pass Infinite Impulse Response filters

To pre-filter element, nodal, contact, integrated, or fastener interaction history output based on one of the low-pass Infinite Impulse Response filters that you defined, you refer to this filter by name from the output request.

Input File Usage:           Use the following option in conjunction with the *ELEMENT OUTPUT, *NODE OUTPUT, *CONTACT OUTPUT, *INTEGRATED OUTPUT, or *INTERACTION OUTPUT options:
*OUTPUT, HISTORY, FILTER=filter_name

ABAQUS/CAE Usage: 

Step module: history output request editor: Apply filter: filter_name


Filtering the output based on the sampling interval

You can request that ABAQUS/Explicit create an anti-aliasing filter internally based on the sampling interval that is specified in the history output request. In this case a filter definition is not required. The anti-aliasing filter is a second order Butterworth type, for which the cutoff frequency is set internally to one-third of the sampling frequency. In this case the sampling frequency is the inverse of the time interval, t, used for the history output.

Input File Usage:           Use the following option in conjunction with the *ELEMENT OUTPUT, *NODE OUTPUT, *CONTACT OUTPUT, *INTEGRATED OUTPUT, or *INTERACTION OUTPUT options:
*OUTPUT, HISTORY, FILTER=ANTIALIASING, TIME INTERVAL=t

ABAQUS/CAE Usage: 

Step module: history output request editor: Save output at every t units of time: Apply filter: Antialiasing


Modal output from ABAQUS/Standard

You can output generalized coordinate (modal amplitude and phase) values during modal dynamic procedures (see Dynamic analysis procedures: overview, Section 6.3.1, for an overview of the modal dynamic procedures available in ABAQUS/Standard) to the output database. Modal output is available only as history output.

Selecting the modal output variables

The modal variables that can be written to the output database are defined in the “Modal variables” section of ABAQUS/Standard output variable identifiers, Section 4.2.1.

Input File Usage:           
*MODAL OUTPUT
list of output variables

ABAQUS/CAE Usage: 

Step module: history output request editor: Select from list below


Controlling the frequency of output

The frequency of modal output is controlled as described above in “Controlling the output frequency in ABAQUS/Standard.”

Requesting output

You can choose to request all modal variables applicable to the current procedure and material type. In this case any additional variables you specify are ignored.

Input File Usage:           
*MODAL OUTPUT, VARIABLE=ALL

ABAQUS/CAE Usage: 

Step module: history output request editor: All


Surface output

You can write variables associated with surfaces in contact, coupled temperature-displacement (ABAQUS/Standard only), coupled thermal-electrical, and crack propagation problems to the output database. The output requests can be repeated as often as necessary within a step to define output for the general contact domain in ABAQUS/Explicit, different contact pair sets, and different types of surface variables.

For surface variables associated with cavity radiation, see “Cavity radiation output in ABAQUS/Standard” below.

Use element output requests (see “Element output”) to obtain database output for contact elements (such as gap elements; see Gap contact elements, Section 31.2.1).

In ABAQUS/Standard contact history output cannot be saved in a linear perturbation step with frequency extraction.

Selecting the surface output variables

The surface variables that can be written to the output database are listed in the “Surface variables” section of ABAQUS/Standard output variable identifiers, Section 4.2.1, and ABAQUS/Explicit output variable identifiers, Section 4.2.2.

Input File Usage:           
*CONTACT OUTPUT
list of output variables

ABAQUS/CAE Usage: 

Step module: field or history output request editor: Select from list below


Selecting the contact pairs for which output is required in ABAQUS/Standard

In ABAQUS/Standard you can select the master and slave surfaces for which output is required, and you can specify a subset of slave nodes for output in addition to the master and slave surfaces or independently. If no surfaces or slave nodes are specified, surface variables are written for all the contact pairs in the model. If you specify the slave surface but not the master surface, output is written for all contact pairs that involve the specified slave surface.

Input File Usage:           
*CONTACT OUTPUT, MASTER=master, SLAVE=slave, NSET=node_set_name

ABAQUS/CAE Usage: 

Step module: field or history output request editor: Domain: Interaction name: contact_interaction_name


Selecting the contact pairs for which output is required in ABAQUS/Explicit

In ABAQUS/Explicit you can select the contact pairs for which surface output is desired. Surface output is contact pair-specific, so that contact output for a particular surface involved in a selected contact pair will include only the contributions from that contact pair if the surface is involved in multiple contact pairs. Surface output is available only for discrete (node-based or element-based) surfaces; it is not available for any analytical surfaces within a contact pair.

Alternatively, you can select the fastened node sets for which output is desired. You cannot select both contact pairs and fastened node sets in the same surface output request.

If no contact pairs or fastened node sets are specified and you do not activate the surface output request for the entire general contact domain (as described below), surface variables are written for all the contact pairs in the model and the general contact domain (if it is defined).

Input File Usage:           Use the following option to request surface output for a particular contact pair:
*CONTACT OUTPUT, CPSET=contact_pair_set_name

Use the following option to request surface output for a particular fastened node set:

*CONTACT OUTPUT, NSET=node_set_name

ABAQUS/CAE Usage: 

Step module: field or history output request editor: Domain: Interaction name: contact_interaction_name


Selecting output for general contact interactions in ABAQUS/Explicit

If the surfaces of a contact pair overlap with the general contact domain, general contact results will still be output for the contact pair surfaces. However, those results exclude contributions from the contact pair interactions.

Field output

You can activate surface output requests for the entire general contact domain. If you do not specify the entire general contact domain or individual contact pairs (as described above), surface variables are written for all the contact pairs in the model and the general contact domain (if it is defined). Surface output for the entire general contact domain is available only as field output.

Input File Usage:           
*CONTACT OUTPUT, GENERAL CONTACT

ABAQUS/CAE Usage: You cannot request surface output for the entire general contact domain in ABAQUS/CAE; you must request history output for a particular surface in the general contact domain, as described below.

History output

You can specify a surface in the general contact domain for which whole surface contact force resultants will be output. Whole surface contact force resultants for a surface in the general contact domain are available only as history output.

Input File Usage:           
*CONTACT OUTPUT, SURFACE=surface_name

ABAQUS/CAE Usage: 

Step module: history output request editor: Domain: General contact surface: surface_name


Controlling the output frequency

The frequency of surface output is controlled as described above in “Controlling the output frequency.”

Requesting preselected output

You can request the preselected, procedure-specific surface output variables described in Table 4.1.3–2. In this case you can specify additional variables as part of the output request.

Alternatively, you can request all surface variables applicable to the current procedure. In this case any additional variables you specify are ignored.

Input File Usage:           Use the following option to request the preselected surface output variables:
*CONTACT OUTPUT, VARIABLE=PRESELECT

Use the following option to request all applicable surface output variables:

*CONTACT OUTPUT, VARIABLE=ALL

ABAQUS/CAE Usage: 

Step module: field or history output request editor: Preselected defaults or All


Time incrementation output in ABAQUS/Explicit

You can output incrementation variables for an ABAQUS/Explicit analysis to the output database. Incrementation output is available only as history output.

Selecting the incrementation output variables

The available incrementation output variables are the ABAQUS/Explicit time increment size, DT; the percent change in mass of the model due to mass scaling, DMASS; and the steady-state detection variables SSPEEQ, SSSPRD, SSFORC, and SSTORQ.

Input File Usage:           
*INCREMENTATION OUTPUT
list of output variables

ABAQUS/CAE Usage: 

Step module: history output request editor: Select from list below


Controlling the output frequency

The frequency of incrementation output is controlled as described above in “Controlling the output frequency for history output in ABAQUS/Explicit.”

Requesting preselected output

You can request the preselected, procedure-specific incrementation output variables. In this case you can specify additional variables as part of the output request.

Alternatively, you can request all incrementation variables applicable to the current procedure type. In this case any additional variables you specify are ignored.

Input File Usage:           Use the following option to request the preselected incrementation output variables:
*INCREMENTATION OUTPUT, VARIABLE=PRESELECT

Use the following option to request all applicable incrementation output variables:

*INCREMENTATION OUTPUT, VARIABLE=ALL

ABAQUS/CAE Usage: 

Step module: history output request editor: Preselected defaults or All


Fastener interaction output

You can write variables associated with fastener interactions (see Mesh-independent fasteners, Section 28.3.4) to the output database. The output request can be repeated as often as necessary to define output for different fastener interactions. Fastener interaction output is available only as history output.

Selecting the fastener interaction output variables

The fastener interaction variables that can be written to the output database are listed in the “Fastener interaction variables” section of ABAQUS/Standard output variable identifiers, Section 4.2.1, and ABAQUS/Explicit output variable identifiers, Section 4.2.2.

Input File Usage:           
*INTERACTION OUTPUT
list of output variables

ABAQUS/CAE Usage: Fastener interaction output cannot be requested in ABAQUS/CAE.

Selecting the fastener interactions for which output is required

You can request output for all fasteners associated with a given fastener interaction or all fasteners associated with a given set of fastener reference nodes.

If you specify a fastener interaction name, the requested output will be written for all fastener layers associated with the specified fastener interaction.

If you specify a node set, any nodes in the node set that are not fastener reference nodes will be ignored.

Input File Usage:           Use the following option to request output for all fasteners associated with a particular fastener interaction:
*INTERACTION OUTPUT, NAME=fastener_interaction_name

Use the following option to request output for all fasteners associated with a particular set of fastener reference nodes:

*INTERACTION OUTPUT,  NSET=node_set_name

ABAQUS/CAE Usage: Fastener interaction output cannot be requested in ABAQUS/CAE.

Controlling the output frequency

The frequency of fastener interaction output is controlled as described above in “Controlling the output frequency.”

Requesting preselected output

There are no preselected variables for fastener interaction output.

Cavity radiation output in ABAQUS/Standard

You can request that cavity-, element-, or surface-based output such as radiation fluxes, viewfactor totals for a facet, and facet temperatures from an ABAQUS/Standard analysis be written to the output database. The output request can be repeated as often as necessary to define output for different variables, different cavities, different element sets, different surfaces, etc.

Selecting the radiation output variables

The radiation output variables that can be written to the output database are listed in the “Cavity radiation variables” section of ABAQUS/Standard output variable identifiers, Section 4.2.1.

Input File Usage:           
*RADIATION OUTPUT
list of output variables

ABAQUS/CAE Usage: Cavity radiation output requests are not supported in ABAQUS/CAE.

Selecting the region of the model for which radiation output is required

You can specify the cavity, element set, or surface for which radiation output is required. Each radiation output request can apply to only one type of region. If you do not specify a region of the model, radiation variables are output for all the cavities in the model.

Input File Usage:           Use one of the following options:
*RADIATION OUTPUT, CAVITY=cavity_name
*RADIATION OUTPUT, ELSET=element_set_name
*RADIATION OUTPUT, SURFACE=surface_name

ABAQUS/CAE Usage: Cavity radiation output requests are not supported in ABAQUS/CAE.

Controlling the output frequency

The frequency of radiation output is controlled as described above in “Controlling the output frequency.”

Requesting output

You can request all radiation variables applicable to the current procedure. In this case any additional variables you specify are ignored.

Input File Usage:           
*RADIATION OUTPUT, VARIABLE=ALL

ABAQUS/CAE Usage: Cavity radiation output requests are not supported in ABAQUS/CAE.

Examples

The examples that follow illustrate how to request multiple types of output over multiple steps in both ABAQUS/Standard and ABAQUS/Explicit.

ABAQUS/Standard example

The input listing below will produce both field and history output for Step 1. Field output will be written every 2 increments. This field output request consists of preselected element variables for the whole model, as well as the variable PEQC. In addition, plastic strains will be written out for element set SMALL, and the nodal variables U and RF will be written to the output database for node set NSMALL. History output will be written every increment. The variables ALLKE, ALLSE, and ALLWK will be written for the whole model. In addition, ALLPD will be written for element set SMALL.

In Step 2 the history output request defined in Step 1 is replaced by a request for the energy variables ALLKE, ALLPD, and ALLSE for element set SMALL. The history output request defined in Step 1 is removed. The field output request defined in Step 1 is passed into Step 2 unchanged, but another field output request for element energies at every increment is added.

*STEP
*STATIC
...
...
*OUTPUT, FIELD, FREQUENCY=2
*ELEMENT OUTPUT, VARIABLE=PRESELECT
PEQC,
*ELEMENT OUTPUT, ELSET=SMALL
PE,
*NODE OUTPUT, NSET=NSMALL
U, RF
*OUTPUT, HISTORY, FREQUENCY=1
*ENERGY OUTPUT
ALLKE, ALLSE, ALLWK
*ENERGY OUTPUT, ELSET=SMALL
ALLPD
*END STEP
*STEP
*STATIC
...
...
*OUTPUT, HISTORY, OP=REPLACE, FREQUENCY=1
*ENERGY OUTPUT, ELSET=SMALL
ALLKE, ALLPD, ALLSE
*OUTPUT, FIELD, OP=ADD, FREQUENCY=1
*ELEMENT OUTPUT
ELEN
*END STEP

ABAQUS/Explicit example

The input listing below will produce both field and history output for Step 1. Field output will be written at 5 equally spaced intervals, and the time marks will be hit exactly. This field output request consists of preselected element variables for the whole model, as well as the variable PEQC. In addition, plastic strains will be written out for element set SMALL, and the nodal variables U and RF will be written to the output database for node set NSMALL. History output will be written at a time interval of 0.005. The ABAQUS/Explicit time step, DT, will be written, along with the variables ALLKE, ALLSE, and ALLWK for the whole model. The output variables SOAREA and SOF integrated over the surface CROSS_SECTION1 will be written. The preselected variables SOF and SOM integrated over the surface CROSS_SECTION2 defined by the integrated output section SECTION1 will be written in the local coordinate system LOCALSYSTEM. In addition, ALLPD will be written for element set SMALL.

In Step 2 the history output request defined in Step 1 is replaced by a request for the energy variables ALLKE, ALLPD, and ALLSE for element set SMALL. The history output request defined in Step 1 is removed. The field output request defined in Step 1 is passed into Step 2 unchanged, but another field output request for element energies at 10 equally spaced intervals is added.

*STEP
*DYNAMIC, EXPLICIT,.1...
...
*OUTPUT, FIELD, NUMBER INTERVAL=5, TIME MARKS=YES
*ELEMENT OUTPUT, VARIABLE=PRESELECT
PEQC,
*ELEMENT OUTPUT, ELSET=SMALL
PE,
*NODE OUTPUT, NSET=NSMALL
U, RF
*OUTPUT, HISTORY, TIME INTERVAL=0.005
*INCREMENTATION OUTPUT
DT
*ENERGY OUTPUT
ALLKE, ALLSE, ALLWK
*ENERGY OUTPUT, ELSET=SMALL
ALLPD
*INTEGRATED OUTPUT, SURFACE=CROSS_SECTION1
SOF, SOAREA
*INTEGRATED OUTPUT SECTION, NAME=SECTION1, 
SURFACE=CROSS_SECTION2, ORIENTATION=LOCALSYSTEM 
*INTEGRATED OUTPUT, SECTION=SECTION1, VARIABLE=PRESELECT 
*END STEP
*STEP
*DYNAMIC, EXPLICIT,.1...
...
*OUTPUT, HISTORY, OP=REPLACE, TIME INTERVAL=0.005
*ENERGY OUTPUT, ELSET=SMALL
ALLKE, ALLPD, ALLSE
*OUTPUT, FIELD, OP=ADD, NUMBER INTERVAL=10
*ELEMENT OUTPUT
ELEN
*END STEP