About Output

You can control the amount of information written to the data file by the analysis input file processor in Abaqus/Standard and Abaqus/Explicit.

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 and Cavity Radiation in Abaqus/Standard. 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). The list of available variables is given in Abaqus/Standard Output Variable Identifiers. Output of results to the data file is requested as part of a step definition.

An Abaqus model can be defined in terms of an assembly of part instances (see Assembly Definition). 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 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 SIM database file (job-name.sim) contains model and results information. The Physics Results Explorerapp on the 3DEXPERIENCE platform uses this database for high-performance postprocessing of analysis results.

You choose the variables to be written to the output database from the lists in Abaqus/Standard Output Variable Identifiers and Abaqus/Explicit Output Variable Identifiers. 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.

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. History output is intended to be output for a small portion of the model requested at a fairly high frequency.

A subset of options in Abaqus/Standard and Abaqus/Explicit are not supported for analyses that produce results 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
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

In Abaqus/Standard you choose the variables to be written to the results file from the lists in Abaqus/Standard Output Variable Identifiers 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 and Cavity Radiation in Abaqus/Standard for details.

The Abaqus/Explicit results file is a sequential access file generated from the selected results file (see Abaqus/Standard and Abaqus/Explicit Execution). The results file contains the requested results in the format described in Results File.

An Abaqus model can be defined in terms of an assembly of part instances (see Assembly Definition). 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.

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.

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

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

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). 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 for an explanation of the output variable types.) Consolidating output variable entries is encouraged, since it will reduce the size of the results file.

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

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.

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.

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 and Contact Diagnostics in an Abaqus/Explicit Analysis).

The Abaqus/Standard 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 status file cannot be controlled.

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 identifier of the element with the smallest stable time increment, 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 and Contact Diagnostics in an Abaqus/Explicit Analysis for details).

Errors that can be detected only while packaging the data for Abaqus/Explicit or during analysis are also written to 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.

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.

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.

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. 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).

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 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).

You can write the element matrix records to the Abaqus/Standard data file.

You can choose to write the load vector from distributed loads on the elements. By default, the load vector is not written.

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.

You can choose to output the stiffness matrix (or operator matrix in heat transfer elements). By default, the stiffness (operator) matrix is not output.

You can choose to output the mass matrix. By default, element mass matrices are not output.

If you use this postprocessing technique to recover additional output from a previous direct cyclic analysis (see Direct Cyclic Analysis), 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.

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), 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.

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