MultiPhysicsVault/.raw/AbaqusAnalysisUserGuide1/AbaqusAnalysisUserGuide1_060.md

3.7.1 FORTRAN UNIT NUMBERS USED BY Abaqus

Products: Abaqus/Standard Abaqus/Explicit

Reference

• “Execution procedure for Abaqus: overview,” Section 3.1.1

Overview

Abaqus uses the Fortran unit numbers outlined in the table below. Unless noted otherwise, you should not try to write to these Fortran units from user subroutines.

For Abaqus/Standard, you should specify unit numbers 15–18 or unit numbers greater than 100 .

For Abaqus/Explicit, specify units 16–18 or unit numbers greater than 100 ending in 5 to 9, e.g. 105, 268, etc. You cannot write to the.sta file.

Fortran unit numbers

Code	Unit Number	Description
Abaqus/Standard	1	Internal database
	2	Solver file
	6	Printed output (.dat) file (You can write output to this file.)
	7	Message (.msg) file (You can write output to this file.)
	8	Results (.fil) file
	10	Internal database
	12	Restart (.res) file
	19–30	Internal databases (scratch files). Unit numbers 21 and 22 are always written to disk.
	73	Text file containing meshed beam cross-section properties (.bsp)

Code	Unit Number	Description
Abaqus/Explicit	6	Printed output (.log) .
	12	Restart (.res) file
	13	Old restart (.res) file, if applicable
	15	Analysis Preprocessor (.dat or .pre) file
	23	Communications (.023) file
	60	Global package (.pac) file
	61	Global state (.abq) file
	62	Temporary file
	63	Global selected results (.sel) file
	64	Message (.msg) file
	65	Output database (.odb) file
	67	Old package (.pac) file, if import from Abaqus/Explicit
	68	Old state (.abq) file, if import from Abaqus/Explicit
	69	Internal database; temporary file
If domain-parallel	70	Local package (.pac.1) file for CPU #1
	71	Local state (.abq.1) file for CPU #1
	73	Local selected results (.sel.1) file for CPU #1
	80	Local package (.pac.2) file for CPU #2
	81	Local state (.abq.2) file for CPU #2
	83	Local selected results (.sel.2) file for CPU #2
	...	Add three files, incrementing units by 10, for each additional CPU

Part II: Output

• Chapter 4, “Output”
• Chapter 5, “File Output Format”

4. Output

Output 4.1

Output variables 4.2

The postprocessing calculator 4.3

4.1 Output

• “Output,” Section 4.1.1
• “Output to the data and results files,” Section 4.1.2
• “Output to the output database,” Section 4.1.3
• “Error indicator output,” Section 4.1.4

4.1.1 OUTPUT

Products: Abaqus/Standard Abaqus/Explicit Abaqus/CFD Abaqus/CAE

References

• “Output to the data and results files,” Section 4.1.2
• “Output to the output database,” Section 4.1.3
• “Abaqus/Standard output variable identifiers,” Section 4.2.1
• “Abaqus/Explicit output variable identifiers,” Section 4.2.2
• “Abaqus/CFD output variable identifiers,” Section 4.2.3
• “Diagnostic printing,” Section 14.5.3 of the Abaqus/CAE User’s Guide
• “Degree of freedom monitor requests,” Section 14.5.4 of the Abaqus/CAE User’s Guide

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.

Abaqus can create files for restarting an analysis—see “Restarting an analysis,” Section 9.1.1. In Abaqus/Standard these files can also be used to extract results output not requested during an analysis.

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 I _ { 3 3 } component corresponding to the only active rotation degree of freedom; the remaining components are not included.