Requesting output for Abaqus analyses

You can create modeling objects to request output from an Abaqus analysis. The output request modeling objects let you specify, for example:

• The types of files that Abaqus creates during the analysis.

• The types of results that Abaqus outputs from the analysis.

• Options that control how Abaqus generates and reports the results. For example, you can control the location at which the software calculates the output variables, such as at the element integration points or centroids.

Once you create an output requests modeling object, you can reuse that output request in any solution step.

In a General step of an Abaqus Structural analysis, you can output different types of results to different types of output files by creating multiple Abaqus Structural Output Requests modeling objects. For example, you can create one modeling object to request output of reaction forces to a data (DAT) file, another modeling object to output stresses to an output database (ODB) file, and a third to output strains to a results (FIL) file. The Abaqus Structural Output Requests modeling objects can also be active in different steps of the solution.

For more information, see Requesting multiple output for Abaqus Structural analyses.

Type of modeling objects

Modeling object	Supports
Abaqus Structural Output Requests	Structural analyses, including requesting output results for explicit analyses: Dynamic Explicit, Axisymmetric Dynamic Explicit, and Dynamic Coupled Thermal-Structural
Abaqus Thermal Output Requests	Thermal
Abaqus Thermal-Structural Output Request	Dynamic Coupled Thermal-Structural and Coupled Thermal-Structural

Supported Abaqus output files

You can generate the following types of Abaqus result files:

• Output database files (ODB), which are neutral binary files that Abaqus uses to store model information and analysis results. You can post-process ODB files.

• Results files (FIL), which you can use for post-processing the results. Note: For Structural analyses, you can specify the format of the results file output, either ASCII or binary, and specify that the output be written at the beginning of a step (the zero increment). You use the Optional Controls tab of the Solution dialog box to set the format and zero increment. For more information, see Solution dialog box (Abaqus).

• Message files (MSG), which are text files that contain diagnostic or informative messages about the progress of the solution. They also contain any errors or warnings.

• Data file (DAT), which contain information about the model and its history.

• Status files (STA), which are text files that contain information about the progress of the analysis. Abaqus writes information to the status file as it performs the analysis. Because you can view the status file while your job is still executing, you can use the status file to monitor the progress of the analysis

Abaqus output variables and options

The tabs at the bottom of the dialog boxes let you select specific output types, as well as options to control each output type. For more information about the dialog box options, see Abaqus Structural, Explicit, Thermal, and Thermal-Structural Output Requests dialog box.

You can specify a broad range of Abaqus output variables, as well as individual components. For example, you can output selected strain components, such as plastic strain (PE) or nominal strain (NE). You can also can output values, such as transverse shear stresses (TSHR) and all failure measure components for laminates (CFAILURE). You can also output specific components of an output variable. By requesting output for only the components you want, the model solves faster and the software produces smaller results files.

For example, you can select any or all of the CSTRESS three output components: CPRESS, CSHEAR1, and CSHEAR2. In addition, you can use All CSTRESS components option to quickly select all components.

You can select the components for stresses, strains, displacements, translations and rotations, reaction forces and moments, and contact displacements.

Note:

Not all components are available in all types of solutions or for all output file types. If you request an output component that is not available for the selected results file type, the software writes the general output variable to the results file. For example, if you select strain components E22 and E13 for output to all results file types, the software writes E (all strain components) to results (FIL) and field output (ODB) files because E22 and E13 are not valid for results (FIL) and field output (ODB) files.

By requesting output for only the components you want, the model solves faster and the software produces smaller results files.

Associated keywords

The Nodal data output cards: *NODE OUTPUT, *NODE FILE, and *NODE PRINT

Element data output cards: *ELEMENT OUTPUT, *EL FILE, and *EL PRINT

Where do I find it?

Application	Pre/Post
Prerequisites	A Simulation file as the work part and displayed partAbaqus as the specified solver
Command Finder	Abaqus Structural Output Requests, Abaqus Thermal Output Requests, or Abaqus Thermal-Structural Output Requests

How do I

Create multiple output requests

Learn more

Requesting multiple output for Abaqus Structural analyses

Requesting output at section points (Abaqus)

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Requesting output for Abaqus analyses, Simcenter 3D 2021.1 Series

© 2020 Siemens

window.mainLanguage="en_US"

window.delivId=""

window.projectId=""

MathJax.Hub.Config({ TeX: { extensions: ["autoload-all.js"] }, tex2jax: { displayMath: [ ] }, "SVG": { scale: 125 } });