4.1.1 Output
Products: Abaqus/Standard Abaqus/Explicit Abaqus/CFD Abaqus/CAE
References
Overview
Abaqus can create the following output files during an analysis:
a data file containing printed output of the model and history definition generated by the analysis input file processor and, in Abaqus/Standard, printed output of results written during the analysis run;
an ODB output database file containing results for postprocessing with the Visualization module of Abaqus/CAE (Abaqus/Viewer) and, in Abaqus/Standard, diagnostic information;
a SIM database file containing results for high-performance postprocessing with the Physics Results Explorer app on the 3DEXPERIENCE platform;
a selected results file in Abaqus/Explicit;
a results file containing results for postprocessing with external software in Abaqus/Standard and Abaqus/Explicit (in Abaqus/Explicit this file is generated by converting the selected results file);
a message file containing diagnostic messages about the solution in Abaqus/Standard and Abaqus/Explicit;
a status file containing information about the status of the analysis and, in Abaqus/Explicit, diagnostic messages and information about the stable time increment; and
output files in Abaqus/CFD using alternate file formats.
The data file
The data file (job-name.dat) is a text file that contains information about the model definition (generated by the analysis input file processor) and, in Abaqus/Standard, tabular output of results. The analysis input file processor information includes the model definition, the history definition, and messages identifying any error and warning conditions that were detected while processing the input data.
Controlling the amount of analysis input file processor information written to the data file
You can control the amount of information written to the data file by the analysis input file processor in Abaqus/Standard and Abaqus/Explicit.
| Input File Usage: | Use the following option in the model definition section of the input file: |
*PREPRINT |
| Abaqus/CAE Usage: | Job module: job editor: General: Preprocessor Printout |
Input file echo
By default, the input file will not be echoed to the data file. You can choose to activate this printout. If the input file is defined in terms of an assembly of part instances, the echo to the data file will be that of the flattened input file (i.e., one that does not use parts and assemblies).
| Input File Usage: | *PREPRINT, ECHO=YES or NO |
| Abaqus/CAE Usage: | Job module: job editor: General: Preprocessor Printout: Print an echo of the input data |
Input parameter information
For parametrized input files, information about input parameters and their values can be printed in the data file. By default, the modified version of the original input file showing this information will not be printed in the data file. You can choose to activate this printout.
| Input File Usage: | *PREPRINT, PARVALUES=YES or NO |
| Abaqus/CAE Usage: | Parametrized input files are not supported in Abaqus/CAE. |
Parameter-free input file information
For parametrized input files, a parameter-free version (after parameter evaluation and substitution) of the original input file can be printed in the data file. By default, this modified version of the input file will not be printed in the data file. You can choose to activate this printout.
| Input File Usage: | *PREPRINT, PARSUBSTITUTION=YES or NO |
| Abaqus/CAE Usage: | Parametrized input files are not supported in Abaqus/CAE. |
Model and history definition summaries
By default, the options defining the model and history data will not be summarized in the data file. You can choose to activate this printout.
For an Abaqus/Explicit analysis the model summary data, when requested, includes the mass, center of mass, and the rotary inertia information for the element sets in the model and for the whole model. However, for two-dimensional models the reported rotary inertia includes the 
component corresponding to the only active rotation degree of freedom; the remaining components are not included.
| 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.
The output database
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 |
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 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:
*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 PARTICLEThe 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
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-electrical-structural 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)
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: |
abaqus job=job-name convert=select abaqus job=job-name convert=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.
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 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 3204and record key 101 for node 135 and 6 degrees of freedom would be written
*I 19I 3101I 3135D1.280271914214298E-10D1.500000000000036E+00 D-1.074629835784448E-46D 6.983222716550941E-12 D-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:
*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.
| Abaqus/CAE Usage: | Step module: Output |
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 |
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 |
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 |
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 |
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 |
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 |
Requesting detailed adaptive mesh smoothing printout
You can activate detailed printout of adaptive mesh smoothing in Abaqus/Standard. The output includes information about the magnitude of the maximum displacement and the node and degree of freedom where the maximum displacement increment occurs during each mesh sweep. It also provides the node numbers at which geometric feature changes occur. By default, only a summary is output.
| Input File Usage: | *PRINT, ADAPTIVE MESH=YES or NO |
| Abaqus/CAE Usage: | Adaptive mesh output to the message file is not supported in Abaqus/CAE. |
Monitoring a degree of freedom in the message file
You can write the current value of a specified point and degree of freedom to the message file. This information can be used to monitor the progress of the solution. The information will also be written in the status file (see below). You can control the frequency at which the value is printed in the message file. The default frequency is 1 (or 10 in a direct cyclic analysis).
Degree of freedom monitoring does not apply to eigenvalue buckling prediction, eigenfrequency extraction, or response spectrum procedures. For other linear perturbation procedures output for the monitored degree of freedom is the base state value.
| Abaqus/CAE Usage: | Step module: Output |
In Abaqus/CAE only one point and degree of freedom can be monitored for an analysis; you cannot change the monitor request from step to step. |
The Abaqus/Explicit message file
In Abaqus/Explicit the message file contains messages if potential problems are detected during an analysis. You can control the output of diagnostic messages for each step (see “Explicit dynamic analysis,” Section 6.3.3, and “Contact diagnostics in an Abaqus/Explicit analysis,” Section 39.2.1). 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).
The status file
The status file (job-name.sta) is a text file that contains information about the progress of an analysis.
The Abaqus/Standard or Abaqus/CFD status file
The Abaqus/Standard or Abaqus/CFD status file contains a single 80-character record for each increment and is updated upon completion of each increment of an analysis. This record is written directly to secondary storage immediately at the completion of the increment. Therefore, the status file can be examined as the analysis job is executing, thus providing a monitor of the progress of the analysis. Other than specifying that a degree-of-freedom variable be monitored in the status file in Abaqus/Standard (as described below), the information written to the Abaqus/Standard or Abaqus/CFD status file cannot be controlled.
The Abaqus/Explicit status file
In Abaqus/Explicit the status file (job-name.sta) contains, by default, mass and inertial properties for the model, initial stable time increment information, a synopsis of the progress of the analysis including total accumulated CPU usage and the current time increment size, and an estimate of the memory required to process each step. You can control additional output including the total kinetic energy, the energy balance, the identifiers of the elements with the smallest stable time increments, and the percent change in total mass of the model due to mass scaling.
The frequency at which summary increments are written to the Abaqus/Explicit status file depends on the duration of the analysis in CPU minutes and the amount of output specified in the analysis. The following list provides general guidelines for when a summary increment will be written to the status file.
Summary information will generally be written:
Each time restart information, field output to the output database, or results file output is written.
Once per increment if the problem requires fewer than 20 increments.
20 times during the step for a short analysis (less than 40 CPU minutes).
Every 2 CPU minutes for an analysis longer than 40 CPU minutes.
A degree-of-freedom variable can be monitored in the status file while the analysis is running. You can also write additional diagnostic information to the status file (see “Explicit dynamic analysis,” Section 6.3.3, and “Contact diagnostics in an Abaqus/Explicit analysis,” Section 39.2.1, for details). A portion of the diagnostic information in the status file, including information for each summary increment, 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).
Errors that can be detected only while packaging the data for Abaqus/Explicit or during analysis are also written to the status file.
| Abaqus/CAE Usage: | Step module: Output |
Requesting kinetic energy output
By default, the kinetic energy for the model is written to the status file. This output is written periodically throughout the step. You can choose to include or exclude the kinetic energy output for each step.
| Input File Usage: | *PRINT, ALLKE=YES or NO |
| Abaqus/CAE Usage: | Step module: Output |
Requesting total energy output
By default, the energy balance is written periodically throughout the step. You can choose to include or exclude the energy balance output for each step.
| Input File Usage: | *PRINT, ETOTAL=YES or NO |
| Abaqus/CAE Usage: | Step module: Output |
Requesting output of the critical element
By default, the number of the element with the current minimum stable time increment and its value are output to the status file. This output is written periodically throughout the step. You can choose to include or exclude the critical element output for each step.
| Input File Usage: | *PRINT, CRITICAL ELEMENT=YES or NO |
| Abaqus/CAE Usage: | Step module: Output |
Requesting output of the change in the total mass
You can write the percent change in total mass of the model due to mass scaling to the status file for each step. This output is written periodically throughout the step. The percent change in total mass is printed by default only if mass scaling is present in the model.
| Input File Usage: | *PRINT, DMASS=YES or NO |
| Abaqus/CAE Usage: | Step module: Output |
Monitoring a degree of freedom in the status file
You can write the current value of a specified point and degree of freedom to the Abaqus/Standard status file. The value of the point and degree of freedom being monitored will appear in the status file for every increment written during the analysis.
When a degree of freedom is monitored in the Abaqus/Standard status file, the same information is written to the message file (see above), but the specified frequency has no effect on the output to the status file.
Degree of freedom monitoring does not apply to eigenvalue buckling prediction, eigenfrequency extraction, or response spectrum procedures. For other linear perturbation procedures output for the monitored degree of freedom is the base state value.
| Abaqus/CAE Usage: | Step module: Output |
In Abaqus/CAE only one point and degree of freedom can be monitored for an analysis; you cannot change the monitor request from step to step. |
Alternate output formats in Abaqus/CFD
By default, when you request output in Abaqus/CFD, the output is sent to the output database file. However, you have the option of selecting alternate file formats for field and history output. History output can be sent to files in comma-separated values (CSV) format instead of the output database formats.
You request the field and history output in the same manner as described in “Requesting output to the output database.” To select an alternate output format, you set the field and history options on the command line when you run an Abaqus/CFD analysis. For more information, see “Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD execution,” Section 3.2.2.
History output in CSV format
The comma-separated values (CSV) format is a text-based output format. The format of the CSV text file consists of one or more comment lines followed by one line of comma-separated data per history output frame. Comments in the CSV file begin with the character #. Each column in the CSV file has a comment that describes the mesh location, the part instance, and the output request label. Possible values for mesh locations are node, element, or surface. Vector output requests also include the component; i.e., 1, 2, or 3.
This format uses file extension csv. History output in the CSV format creates one file per output request label per step. Additional files are created if the job is run in parallel and the set associated with the history output request is split between processors due to the domain decomposition. In this case there will be one file per processor on which the set is present. The files are named job_output-request_rank_step-number.csv, where rank is a number ranging from 0 to one less than the number of CPUs.
| Input File Usage: | Use the following command line option to write history output to an alternate file format in Abaqus/CFD: |
abaqus job=job-name history=csv |
| Abaqus/CAE Usage: | You cannot select an alternate format for history output in Abaqus/CAE. |
Requesting output in multiple steps
In general, output requests apply to the step in which they are given and to all subsequent steps until they are respecified. However, output specifications for linear perturbation steps (available only in Abaqus/Standard; see below and “General and linear perturbation procedures,” Section 6.1.3) are treated independently of output requests for general analysis steps and apply only to a continuous sequence of linear perturbation steps.
Database output, printed output, and results file output are independent output modes in Abaqus; therefore, changing the specification for one form of output does not affect the other forms.
General analysis steps
The default output requests are used in the first general analysis step of an analysis unless you redefine them. For subsequent general analysis steps, the definition of each form of output from the previous general step is maintained unless you redefine it.
Linear perturbation steps
The default output requests are used in the first of any sequence of linear perturbation steps unless they are redefined in that step. If a subsequent linear perturbation step is defined without an intermediate general analysis step, the definition of each mode of output from the previous perturbation step is maintained unless you redefine it. If an intermediate general step is defined, the default output requests are again used in the linear perturbation step unless they are redefined in that step.
Element matrix output in Abaqus/Standard
In Abaqus/Standard you can write element stiffness matrices and, if available, mass matrices for each step to a file. For heat transfer elements the operator matrices are written if stiffness matrix output is requested.
Element matrix output is available only for elements without internal nodes (unless those nodes have no active degrees of freedom) and with no acoustic or internal degrees of freedom. Examples of elements for which element matrix output is prohibited include acoustic, pipe, elbow, frame, gap, and interface elements as well as axisymmetric elements with Fourier modes. Element matrix output is not available for elements with coupled fields such as coupled temperature-displacement elements and pore pressure elements. For incompatible mode and hybrid elements, stiffness matrix output is prohibited while mass matrix output is available. A substructure matrix output request is used to write a substructure's reduced stiffness matrix, mass matrix, and load case vectors to a file (see “Defining substructures,” Section 10.1.2).
Element matrix output cannot be requested in a mode-based dynamic analysis (response spectrum, steady-state dynamic, modal dynamic, or random response). However, it can be requested in the eigenfrequency extraction analysis that precedes the mode-based dynamic analysis to output the mass and stiffness matrices.
The element matrices are written without the effects of nodal conditions; therefore, boundary conditions, concentrated loads, and the effects of multi-point constraints are not included in this output. The degrees of freedom are always in the global directions, even if a local coordinate system (“Transformed coordinate systems,” Section 2.1.5) has been defined at nodes associated with the element.
You must select the element set for which output is requested. For models defined in terms of an assembly of part instances (“Defining an assembly,” Section 2.10.1), element numbers written with element matrix output are internal numbers generated by Abaqus/Standard. A map between internal numbers and the original element numbers and part instance names is provided in the data file.
Writing the element matrices to the results file
By default, element matrix output records are written to the Abaqus/Standard results file. The record formats for the results file are described in “Results file output format,” Section 5.1.2. The file can be written in binary or ASCII format based on the file format you specify (see “Controlling the format of the results file in Abaqus/Standard” above).
| Input File Usage: | *ELEMENT MATRIX OUTPUT, ELSET=element_set, OUTPUT FILE=RESULTS FILE |
| Abaqus/CAE Usage: | Element matrix output is not supported in Abaqus/CAE. |
Writing the element matrices to a user-defined file
You can write the element matrices to a user-defined file. The file name should not include an extension; the extension .mtx will be added. (See “Input syntax rules,” Section 1.2.1, for the syntax of user-specified file names.)
The format of the output file is compatible with the linear user element (see “User-defined elements,” Section 32.17.1).
| Input File Usage: | *ELEMENT MATRIX OUTPUT, ELSET=elset, OUTPUT FILE=USER DEFINED, FILE NAME=output_file_name |
| Abaqus/CAE Usage: | Element matrix output is not supported in Abaqus/CAE. |
Writing the element matrices to the data file
You can write the element matrix records to the Abaqus/Standard data file.
| Input File Usage: | *ELEMENT MATRIX OUTPUT, ELSET=elset, OUTPUT FILE=USER DEFINED |
| Abaqus/CAE Usage: | Element matrix output is not supported in Abaqus/CAE. |
Including distributed loads
You can choose to write the load vector from distributed loads on the elements. By default, the load vector is not written.
| Input File Usage: | *ELEMENT MATRIX OUTPUT, ELSET=elset, DLOAD=YES or NO |
| Abaqus/CAE Usage: | Element matrix output is not supported in Abaqus/CAE. |
Controlling the frequency of element matrix output
You can control the frequency at which element matrix output will be written by specifying an output frequency in increments. By default, the element matrices will be output every increment (equivalent to an output frequency of 1). Specify an output frequency of 0 to suppress output of the element matrices. Unless the output is suppressed, the matrices will always be written at the last increment of a step.
| Input File Usage: | *ELEMENT MATRIX OUTPUT, ELSET=elset, FREQUENCY=N |
| Abaqus/CAE Usage: | Element matrix output is not supported in Abaqus/CAE. |
Writing the stiffness or operator matrix
You can choose to output the stiffness matrix (or operator matrix in heat transfer elements). By default, the stiffness (operator) matrix is not output.
| Input File Usage: | *ELEMENT MATRIX OUTPUT, ELSET=elset, STIFFNESS=YES or NO |
| Abaqus/CAE Usage: | Element matrix output is not supported in Abaqus/CAE. |
Writing the mass matrix
You can choose to output the mass matrix. By default, element mass matrices are not output.
| Input File Usage: | *ELEMENT MATRIX OUTPUT, ELSET=elset, MASS=YES or NO |
| Abaqus/CAE Usage: | Element matrix output is not supported in Abaqus/CAE. |
User-defined output variables in Abaqus/Standard
In Abaqus/Standard output quantities can be defined as functions of any element integration point variable listed in “Abaqus/Standard output variable identifiers,” Section 4.2.1, by using user subroutine UVARM. Then, output variable UVARMn can be requested for output to the data file, the results file, or the output database.
User-defined state variables in Abaqus/Standard
In Abaqus/Standard you can allocate solution-dependent state variables and define them in user subroutines defining material behavior, as well as user subroutines FRIC, UEL, and UINTER (see “User subroutines: overview,” Section 18.1.1). Output variable SDVn can be requested for output of these state variables to the data file, the results file, or the output database. For user-defined elements output variable SDVn cannot be requested for output to the output database.
Postprocessing with Abaqus/CAE
Abaqus/CAE provides interactive graphical postprocessing from the Abaqus output database file in the Visualization module (also licensed separately as Abaqus/Viewer). Capabilities include model and deformed shape plotting, contour plotting, vector plotting, X–Y plotting, and animation.
Recovering additional results output from restart data in Abaqus/Standard
Data needed for restart in Abaqus/Standard are contained in several files that are generated when you request that restart data be written for an analysis: the restart (.res), analysis database (.mdl and .stt), part (.prt), and output database (.odb) files. “Restarting an analysis,” Section 9.1.1, describes the writing of restart data in more detail.
In Abaqus/Standard you can extract output from the restart data and write it to new data (.dat), results (.fil), and output database (.odb) files using a postprocessing analysis procedure. If the original analysis included user subroutines, the postprocessing analysis procedure requires the specification of the user subroutines. The data, results, and output database file output requests are defined as described in “Output to the data and results files,” Section 4.1.2, and “Output to the output database,” Section 4.1.3. The output requests should be defined exactly as they would be in an analysis, except that:
The output frequency specification has no meaning and is, therefore, ignored (unless you are recovering additional output from a previous direct cyclic or low-cycle fatigue analysis). Instead, you specify each increment at which output is to be generated in the postprocessing procedure definition.
No default output is provided to the output database. Furthermore, model information, such as boundary conditions, is not written to the output database.
Element set energy information cannot be recovered since it is not written to the restart file.
Output is not available for procedures that do not support restart; for example, linear perturbation procedures.
| Input File Usage: | *POST OUTPUT, STEP=step_number |
When the *POST OUTPUT option is used, it must appear as the first option in the input file. No data lines from the analysis input file are required. This option can be repeated as often as necessary to obtain further output. Since *POST OUTPUT is a purely postprocessing procedure, analysis options must not appear in the input file. |
| Abaqus/CAE Usage: | Postprocessing of restart data is not supported in Abaqus/CAE. |
Recovering additional output from a direct cyclic analysis
If you use this postprocessing technique to recover additional output from a previous direct cyclic analysis (see “Direct cyclic analysis,” Section 6.2.6), you must specify the iteration number in the restart file from which output is required instead of the increment. If temperatures (or predefined field variables) are read from a results (.fil) file in the original direct cyclic analysis, the same temperatures (or predefined field variables) must be read into the postprocessing analysis. This specification is needed to recover thermal strains at each time increment in the original direct cyclic analysis since the results file is not stored in the restart analysis database.
| Input File Usage: | *POST OUTPUT, STEP=step_number, ITERATION=iteration_number |
There are no data lines associated with this option if the ITERATION parameter is specified. |
| Abaqus/CAE Usage: | Postprocessing of restart data is not supported in Abaqus/CAE. |
Recovering additional output from a low-cycle fatigue analysis
If you use this postprocessing technique to recover additional output from a previous low-cycle fatigue analysis (see “Low-cycle fatigue analysis using the direct cyclic approach,” Section 6.2.7), you must specify the cycle number in the restart file from which output is required instead of the increment. If temperatures (or predefined field variables) are read from a results (.fil) file in the original low-cycle fatigue analysis, the same temperatures (or predefined field variables) must be read into the postprocessing analysis. This specification is needed to recover thermal strains at each time increment in the original low-cycle fatigue analysis since the results file is not stored in the restart analysis database.
| Input File Usage: | *POST OUTPUT, STEP=step_number, CYCLE=cycle_number |
There are no data lines associated with this option if the CYCLE parameter is specified. |
| Abaqus/CAE Usage: | Postprocessing of restart data is not supported in Abaqus/CAE. |
Example
A job can be submitted using the following input file. The analysis for which restart data were written must be specified when you submit the job (using the oldjob parameter of the Abaqus execution procedure). This example creates a new data (.dat) file containing tabular data. The first two tables will contain data from increments 5 and 10 of Step 1 and will give the reaction forces of the nodes in the set CLAMP, which was defined when the analysis was run. The next table will contain data from increment 3 of Step 2 and will give displacements from the new node set TIP that is defined in this postprocessing analysis.
*HEADING *POST OUTPUT, STEP=1 5, 10 *NODE PRINT, NSET=CLAMP RF, *POST OUTPUT, STEP=2 3, *NSET, NSET=TIP 1200, 1203, 1205 *NODE PRINT, NSET=TIP U,
The following example input file recovers additional output from a previous direct cyclic analysis and creates a new output database (.odb) file, which contains the stress and strain for the elements in the set ELIST from each increment in Iteration 5 of Step 1, followed by data from each increment in Iteration 10 of Step 1:
*HEADING *POST OUTPUT, STEP=1, ITERATION=5 *OUTPUT, HISTORY *ELEMENT OUTPUT, ELSET=ELIST S,E *POST OUTPUT, STEP=1, ITERATION=10 *OUTPUT, HISTORY *ELEMENT OUTPUT, ELSET=ELIST S,E
The following example input file recovers additional output from a previous low-cycle fatigue analysis and creates a new output database (.odb) file, which contains the stress and strain for the elements in the set ELIST from each increment in Cycle 5 of Step 1, followed by data from each increment in Cycle 10 of Step 1:
*HEADING *POST OUTPUT, STEP=1, CYCLE=5 *OUTPUT, HISTORY *ELEMENT OUTPUT, ELSET=ELIST S,E *POST OUTPUT, STEP=1, CYCLE=10 *OUTPUT, HISTORY *ELEMENT OUTPUT, ELSET=ELIST S,E