<!-- source-page: 601 -->

Input File Usage: \*PREPRINT, MODEL=YES or NO, HISTORY=YES or NO

Abaqus/CAE Usage: Job module: job editor: General: Preprocessor Printout: Print model definition data and Print history data

# Contact constraint information

In Abaqus/Standard you can choose to activate printout of detailed information about the contact constraints generated by the contact pair definition data.

Input File Usage: \*PREPRINT, CONTACT=YES or NO

Abaqus/CAE Usage: Job module: job editor: General: Preprocessor Printout: Print contact constraint data

# Mass information

In Abaqus/Explicit you can choose to activate printout of detailed information about the mass property of each user-defined element set.

Input File Usage: \*PREPRINT, MASS PROPERTY=YES or NO

Abaqus/CAE Usage: This parameter is not supported by Abaqus/CAE.

# Requesting printed results

In Abaqus/Standard the values of output variables can be printed to the data file in tabular format throughout the analysis. You can control the following types of printed output during the analysis run: element output, node output, contact surface output, energy output, fastener interaction output, modal output, section output, and radiation output—see “Output to the data and results files,” Section 4.1.2, and “Cavity radiation,” Section 41.1.1. You specify the variables to be printed in each output table and, for element variables, the locations at which they are to be printed (at the integration points, at the element centroid, at the nodes, or averaged at the nodes). Nodal variables at nodes with transformations can be written in either the global or the local coordinate system (see “Transformed coordinate systems,” Section 2.1.5). The list of available variables is given in “Abaqus/Standard output variable identifiers,” Section 4.2.1. Output of results to the data file is requested as part of a step definition.

# Viewing part and assembly information in the data file

An Abaqus model can be defined in terms of an assembly of part instances (see “Defining an assembly,” Section 2.10.1). In such a model node and element numbers can be repeated within the definitions of different parts. These local numbers are converted internally by Abaqus to unique global numbers, and the output written to the data file is given in terms of those internal numbers. A map between user-defined numbers and internal numbers is printed to the data file (after the step data) if any output that includes node and element numbers is requested in the data file.

Set and surface names that appear in the data file are prefixed by the assembly and part instance names, separated by underscores (Assembly\_Part1–1\_setname, for example).

Local coordinate systems defined within a part or part instance are translated and rotated according to the positioning data given in the part instance definition.

<!-- source-page: 602 -->

The output database is a neutral binary file. Unlike the restart or binary results files, it can be copied directly from one computing platform to another without translation.

# Format of the output database

The Abaqus output database is available in two formats, ODB and SIM. By default, the results output is created in ODB format. For an Abaqus/Standard or Abaqus/Explicit analysis you have the option to write results in both formats during the same job. Only results in SIM format can be imported into the 3DEXPERIENCE platform for high-performance postprocessing. For more information, see “Limitations when writing and postprocessing results in SIM format” below.

• The ODB output database (job-name.odb) is used to store model information and analysis results in terms of an assembly of part instances. The Visualization module of Abaqus/CAE (Abaqus/Viewer) uses this output database for postprocessing analysis results and viewing diagnostic information.   
• The SIM database file (job-name.sim) contains model and results information. The Physics Results Explorer app on the 3DEXPERIENCE platform uses this database for high-performance postprocessing of analysis results.

Input File Usage: Use the following command line options to write results in an Abaqus/Standard or Abaqus/Explicit analysis in SIM format:

abaqus job=job-name resultsformat=sim

Use the following command line options to write results in an Abaqus/Standard or Abaqus/Explicit analysis in ODB format and in SIM format:

abaqus job=job-name resultsformat=both

Use the following command line options to write field output results in an Abaqus/CFD analysis in SIM format:

abaqus job=job-name field=sim

Use the following command line options to write history output results in an Abaqus/CFD analysis in SIM format:

abaqus job=job-name history=sim

Abaqus/CAE Usage: Use the following input to write results in an Abaqus analysis in SIM format:

Job module: job editor: General: Results Format: SIM

Use the following input to write results in an Abaqus/Standard or Abaqus/Explicit analysis in ODB format and in SIM format:

Job module: job editor: General: Results Format: Both

<!-- source-page: 603 -->

# Handling of floating point data

By default, floating point data are written in single precision to the ODB output database file. You can choose to write floating point nodal field output data to the ODB output database file in double precision; see “Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD execution,” Section 3.2.2, for details.

For Abaqus/Standard and Abaqus/Explicit analyses, floating point data are written to the SIM database in single precision, with the exception of nodal coordinates, which are written in double precision. For Abaqus/CFD analyses, floating point data are written to the SIM database in double precision.

# Opening an output database in Abaqus/CAE

You can open an output database file from an older release of Abaqus in Abaqus/CAE. Output database files from previous releases of Abaqus must be converted to the current release when they are opened. If you are using an older release of Abaqus/CAE, you cannot open an output database file created from a newer release of Abaqus.

# Choosing an output format

Your choice of output format depends on your level of experience with high-performance visualization, the Physics Results Explorer app, and your postprocessing needs.

• If you are still learning to use high-performance visualization and you want to compare your results with Abaqus/Viewer, write results in both formats.   
• If the model is large and you need the improved performance of the Physics Results Explorer app, as well as the capabilities of Abaqus/Viewer, write results in both formats.   
• If you are confident that the high-performance visualization features in the Physics Results Explorer app provide all the capabilities you need, write results in SIM format.

# Requesting output to the output database

You choose the variables to be written to the output database from the lists in “Abaqus/Standard output variable identifiers,” Section 4.2.1, “Abaqus/Explicit output variable identifiers,” Section 4.2.2, and “Abaqus/CFD output variable identifiers,” Section 4.2.3. The following types of output are available: element output, node output, contact surface output, energy output, integrated output, time incrementation output, fastener interaction output, modal output, and radiation output. In addition, a subset of the diagnostic information that is written to the message file in Abaqus/Standard and Abaqus/Explicit (see “The message file in Abaqus/Standard and Abaqus/Explicit”) and to the Abaqus/Explicit status file (see “The status file”) is included in the output database. See “Output to the output database,” Section 4.1.3, for a detailed explanation of how to generate output database requests.

Three types of information are stored in the output database: “field” output, “history” output, and diagnostic information. Field output is intended to be relatively infrequent output for a large portion of the model. Abaqus/CAE uses field output to generate contour plots, displaced shape plots, symbol plots, and X–Y plots in the Visualization module. History output is intended to be output for a small portion of the model requested at a fairly high frequency. Abaqus/CAE uses history output to generate X–Y plots in

<!-- source-page: 604 -->

the Visualization module. See “Output to the output database,” Section 4.1.3, for detailed descriptions of field and history output. Diagnostic information is intended to provide convergence information for use in Abaqus/CAE; for more information, see Chapter 41, “Viewing diagnostic output,” of the Abaqus/CAE User’s Guide.

# Limitations when writing and postprocessing results in SIM format

A subset of options in Abaqus/Standard and Abaqus/Explicit are not supported for analyses that produce results in SIM format; Abaqus/CFD has no restrictions on output in SIM format. If you include one or more of these options or parameters in your analysis and write output in SIM format or both formats, the analysis will either terminate with errors or produce limited results.

The following options produce error messages in the data (.dat) file:

```txt
*ADAPTIVE MESH REFINEMENT
*CONTOUR INTEGRAL
*DIRECT CYCLIC, FATIGUE
*ELECTROMAGNETIC
*ENRICHMENT
*ENRICHMENT ACTIVATION (for XFEM)
*IMPORT
*MAP SOLUTION
*MAGNETOSTATIC
*NMAP, FATIGUE=BLENDED or TOROIDAL
*POST OUTPUT
*REBAR
*SUBSTRUCTURE PATH
*SUBSTRUCTURE DIRECTORY
*SURFACE, TYPE=(EULERIAN MATERIAL, XFEM, BSPLINE, BEZIER, or USER)
*STEADY STATE TRANSPORT
*SYMMETRIC MODEL GENERATION
*SYMMETRIC RESULTS TRANSFER
*TRACER PARTICLE 
```

The following option produces limited results but no error messages:

\*EULERIAN SECTION: some volume fraction data are not written to the SIM database

In addition, the following option produces results in SIM format; however, the results are not accounted for in the Physics Results Explorer app:

\*MODEL CHANGE

<!-- source-page: 605 -->

# The selected results file

The Abaqus/Explicit selected results file (job-name.sel) stores user-selected results, which are converted into the results file (job-name.fil) for postprocessing by other commercial postprocessing packages.

Element output, node output, and energy output can be requested (see “Output to the data and results files,” Section 4.1.2, for details); the variables available for output are listed in “Abaqus/Explicit output variable identifiers,” Section 4.2.2. You can write a user-selected subset of the results for a given node set or element set at more frequent intervals than the restart intervals. You specify the output requests within a step definition, which allows you to be selective about the amount of data written to the selected results file to avoid using excessive disk storage. For example, when dealing with a very large model, you may choose to write only the current displacements and the equivalent plastic strain for the entire model 20 times in the step and to write the acceleration history at one node 200 times in the step.

# The results file

The Abaqus results file in Abaqus/Standard and Abaqus/Explicit (job-name.fil) can be read by external postprocessors to produce X–Y plots or printed tabular output. Most commercial finite element results-display packages provide translators that use the Abaqus results file as their input. The results file can also be used as a convenient medium for importing analysis results into your own postprocessing program. “Accessing the results file information,” Section 5.1.3, provides details on how to read this file.

Results file output of temperature from a heat transfer, thermal-electrical, or thermal-electricalstructural analysis can be used as input to a stress analysis of the same mesh (see “Sequentially coupled thermal-stress analysis,” Section 16.1.2).

# Obtaining results file output in Abaqus/Standard

In Abaqus/Standard you choose the variables to be written to the results file from the lists in “Abaqus/Standard output variable identifiers,” Section 4.2.1, in a manner similar to that for output printed to the data file. You must specifically request that values be written to the results file or none will be provided. Element output, node output, contact surface output, energy output, modal output, and radiation output are available—see “Output to the data and results files,” Section 4.1.2, and “Cavity radiation,” Section 41.1.1, for details.

# Obtaining results at the beginning of a step

You can request that the solution state at the beginning of a step (the zero increment) be written to the Abaqus/Standard results file. Zero-increment file output is available only for steps in which the concept of time governs the incrementation scheme of the selected procedure and, hence, the following procedures are excluded:

• Linear static perturbation analysis (“Static stress analysis,” Section 6.2.2)   
• “Eigenvalue buckling prediction,” Section 6.2.3

<!-- source-page: 606 -->

• “Natural frequency extraction,” Section 6.3.5   
• “Mode-based steady-state dynamic analysis,” Section 6.3.8   
• “Response spectrum analysis,” Section 6.3.10   
• “Random response analysis,” Section 6.3.11

If you request zero-increment results file output, it will be generated for all valid procedures in a given analysis.

You must request zero-increment results file output to generate a zero-increment results file in a data check analysis (see “Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD execution,” Section 3.2.2). It is strongly recommended that you request zero-increment results file output if the results file is used to drive a submodel; see “Node-based submodeling,” Section 10.2.2, for further discussion.

Input File Usage: \*FILE FORMAT, ZERO INCREMENT

The \*FILE FORMAT option can be given as model data or as history data, but it can appear only once in the input file.

Abaqus/CAE Usage: Results file output cannot be requested in Abaqus/CAE.

# Obtaining results file output in Abaqus/Explicit

The Abaqus/Explicit results file is a sequential access file generated from the selected results file (see “Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD execution,” Section 3.2.2). The results file contains the requested results in the format described in “Results file output format,” Section 5.1.2.

Input File Usage: Use either of the following command line options to convert a selected results file to a results file:

$$
\text {   abaqus   job   } = \text {   job   -   name   convert   } = \text {   select   }
$$

$$
\text {   abaqus   job   } = \text {   job   -   name   convert   } = \text {   all   }
$$

Abaqus/CAE Usage: The selected results file cannot be converted in Abaqus/CAE.

# Part and assembly information

An Abaqus model can be defined in terms of an assembly of part instances (see “Defining an assembly,” Section 2.10.1). However, the results file does not contain part and assembly records.

In a model defined in terms of an assembly of part instances, node and element numbers can be repeated within the definitions of different parts. These local numbers are converted internally by Abaqus to unique global numbers, and the output written to the results file is given in terms of the global (internal) numbers. A map between user-defined numbers and internal numbers is printed to the data file if any results file output that includes node and element numbers is requested.

Set and surface names that appear in the results file are prefixed by the assembly and part instance names, separated by underscores (Assembly\_Part1–1\_setname, for example).

Local coordinate systems defined within a part or part instance are translated and rotated according to the positioning data given in the part instance definition.

<!-- source-page: 607 -->

# Format of the results file

The Abaqus results file in Abaqus/Standard or Abaqus/Explicit is organized as a sequential file, in binary or in ASCII format. ASCII format is necessary if the file is to be read on a computer system that is different from the one on which the file was written. ASCII format allows the results file to be transferred between different computer systems without having to translate binary data. ASCII format is not needed if the file will always be used on the same system or on systems that use the same binary format. If the results file output will always reside on the same computer, the default binary format is usually the most efficient way of storing the file. For large problems a file in ASCII format will be significantly larger than the same file in binary format.

# Controlling the format of the results file in Abaqus/Standard

Abaqus/Standard can write the results file in either binary or ASCII format. The default format is binary.

The results file output must be written in the same format for the entire analysis. The format cannot be changed upon restarting the problem.

The format of the Abaqus/Standard results file can also be controlled in the Abaqus/Standard environment file (see “Using the Abaqus environment settings,” Section 3.3.1). The format specified in an analysis supersedes the value defined in the enviroment file.

In addition, the ascfil facility in the Abaqus execution procedure (“ASCII translation of results (.fil) files,” Section 3.2.14) can be used to convert a binary Abaqus/Standard results file (job-name.fil) to ASCII format (job-name.fin) after the analysis completes.

Input File Usage: \*FILE FORMAT, ASCII

The \*FILE FORMAT option can be given as model data or as history data, but it can appear only once in the input file.

Abaqus/CAE Usage: Results file output cannot be requested in Abaqus/CAE.

# Controlling the format of the results file in Abaqus/Explicit

Abaqus/Explicit always writes the results file output in binary format during file conversion, but the binary Abaqus/Explicit results file can be converted to ASCII format using the ascfil facility (“ASCII translation of results (.fil) files,” Section 3.2.14).

# ASCII format

“Results file output format,” Section 5.1.2, defines the contents of the records that are written to the results file; these descriptions also hold if the results file is written in ASCII format. All the data items in these files are either integers, floating point numbers, or character strings. When ASCII format is requested, each data item is translated into an equivalent character string before it is written to the file. These strings are written in 80-character logical records in the order described in the record definitions.

Each 80-character logical record is completely filled before the next one is started, so that any data item can be split, with some of the characters that define the item in one logical record and the remainder in the next. Each data item usually follows immediately behind its predecessor. The exception is that for results file record key 2001 Abaqus will fill out the logical record with blank characters, so that the

<!-- source-page: 608 -->

record can be written immediately to the physical storage medium. Abaqus then inserts a logical record consisting of 80 blanks, which allows the end-of-file to be handled correctly.

The beginning of each “record” is indicated by an asterisk (\*). Each floating point number begins with the character D, followed by the number in the format E22.15 or D22.15, depending on whether the release of Abaqus that wrote the results file used single precision or double precision. Each character string begins with the character A, followed by eight characters (if the character string has fewer than eight characters, the right part of the string is blank; character strings longer than eight characters are written eight characters at a time). Each integer begins with the character I, followed by a two digit integer giving the number of decimal digits in the integer, followed by the integer itself (written as decimal digits).

For example, record key 1900 for an S4R element with element number 5 and nodes 195, 198, 205, and 204 would be written

\*I 18I 41900I 15AS4R I 3195I 3198I 3205I 3204

and record key 101 for node 135 and 6 degrees of freedom would be written

\*I 19I 3101I 3135D1.280271914214298E-10D1.500000000000036E+00D-1.074629835784448E-46D 6.983222716550941E-12D-4.084928798492785E-13D-1.072688441364597E-10

# Precision of floating point data in the results file

The precision of floating point data written to the results file depends on the precision of the executable that generates the data. Abaqus/Standard always uses double precision; thus, floating point data are always written to the Abaqus/Standard results file in double precision. Abaqus/Explicit can be run in single or double precision on most machines; see “Defining an analysis,” Section 6.1.2, for details on the precision level of the Abaqus/Explicit executable. If the double precision executable for Abaqus/Explicit is used, floating point data are written to the Abaqus/Explicit results file in double precision; likewise, if the single precision executable for Abaqus/Explicit is used, floating point data are written to the Abaqus/Explicit results file in single precision.

# Maximizing the efficiency of the results file

In Abaqus/Standard each element output request (a collection of identifying keys entered on a single line) is preceded by an “element header” record (see “Results file output format,” Section 5.1.2). Hence, the size of the results file can be minimized by entering all element output variables of the same “type” (element integration point variable, element section variable, whole element variable, etc.) on a single line. (See “Output to the data and results files,” Section 4.1.2, for an explanation of the output variable types.) Consolidating output variable entries is encouraged, since it will reduce the size of the results file.

# Example

For example, the following output requests can be used to request output of element variables in the results file in a stress/displacement analysis:

<!-- source-page: 609 -->

```csv
*EL FILE
S, SINV, E, PE, CE, EE, ENER, TEMP, FV, COORD
SF, SE
LOADS, ELEN, EVOL
*EL FILE, REBAR
S, SINV, E, PE, CE, EE, RBFOR, RBANG
SF, SE
LOADS, ELEN 
```

(The output requests for rebar quantities need not be the same as the underlying element output requests.)

# The message file in Abaqus/Standard and Abaqus/Explicit

The message file (job-name.msg) is a text file that contains diagnostic messages about the progress of the solution.

# The Abaqus/Standard message file

In Abaqus/Standard the message file contains diagnostic or informative messages about the progress of the solution. If any of these messages describe errors or warnings, the number of such errors or warnings is also given at the end of the data file. The message file is written automatically during an Abaqus/Standard analysis.

The Abaqus/Standard message file contains information about the increment number, step time, fraction of a step completed, equilibrium iterations, severe discontinuity (contact) iterations, plasticity algorithms, adaptive mesh smoothing, the load proportionality factor in a Riks analysis, etc. A portion of the diagnostic information in the message file is also written to the output database for use in Abaqus/CAE (for more information, see “Requesting diagnostic information in Abaqus/Standard and Abaqus/Explicit” in “Output to the output database,” Section 4.1.3).

You can control the amount of information written to the message file for each step. This feature is sometimes helpful in difficult analyses since it allows detailed diagnostic information to be written about certain events (such as contact) during a nonlinear solution; this information can often be useful in developing a strategy for the solution of highly nonlinear problems.

Input File Usage: \*PRINT

The \*PRINT option can appear only once within a step definition.

Abaqus/CAE Usage: Step module: Output→Diagnostic Print

Controlling the frequency of output to the message file

You can control the frequency at which information is printed to the message file by specifying the desired output frequency in increments. The default output frequency is 1 (or 10 in a direct cyclic or a low-cycle fatigue analysis). The output will always be printed at the last increment of each step unless you specify a frequency of zero to suppress the output.

Input File Usage: \*PRINT, FREQUENCY=N

Abaqus/CAE Usage: Step module: Output→Diagnostic Print: Frequency N

<!-- source-page: 610 -->

# Requesting detailed contact printout

You can obtain a detailed printout of contact conditions during iteration. This information about which points are contacting or separating in interface and gap problems is useful in tracking the development of the solution in difficult contact problems. The details are written for every severe discontinuity iteration. By default, the detailed contact output is suppressed.

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

Abaqus/CAE Usage: Step module: Output→Diagnostic Print: toggle on Contact

# Requesting detailed model change printout

You can obtain a detailed printout of model change operations (removal and reactivation) at the start of a step. This information includes the new original coordinates and normals of elements being reactivated strain free in a large-displacement analysis. By default, the detailed model change output is suppressed. See “Element and contact pair removal and reactivation,” Section 11.2.1, for details on model change operations.

Input File Usage: \*PRINT, MODEL CHANGE=YES or NO

Abaqus/CAE Usage: Step module: Output→Diagnostic Print: toggle on Model Change

# Requesting detailed printout of problems with the plasticity algorithms

You can activate printout of element and integration point numbers for which the plasticity algorithms have failed to converge during an iteration. This information is useful for finding the place in the mesh and/or the plasticity model at which Abaqus is encountering material model difficulties. Modeling problems and material parameter specification problems can be identified using this detailed printout. By default, this printout is suppressed.

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

Abaqus/CAE Usage: Step module: Output→Diagnostic Print: toggle on Plasticity

# Requesting output of equilibrium residuals

By default, equilibrium residuals during equilibrium iterations are output. You can choose to suppress this output entirely, but it is not recommended; without the output of equilibrium residuals, you cannot see the accuracy of the iteration process.

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

Abaqus/CAE Usage: Step module: Output→Diagnostic Print: toggle on Residual

# Requesting solver information

By default, information about the number of equations being solved and the number of floating point operations is output for each iteration. You can request for this output to be suppressed.

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

Abaqus/CAE Usage: Step module: Output→Diagnostic Print: toggle on Solve
