2.4 Checking the input data

Having generated the input file for this simulation, you are ready to run the analysis. Unfortunately, it is possible to have errors in the input file because of typing errors or incorrect or missing data. You should perform a datacheck analysis first before running the simulation. To run a datacheck analysis, make sure that you are in the directory where the input file frame_xpl.inp is located, and type the following command:

abaqus job=frame_xpl datacheck interactive

If this command results in an error message, the ABAQUS installation on your computer has been customized. You should contact your systems administrator to find out the appropriate command to run ABAQUS. The job=frame_xpl parameter specifies that the jobname for this analysis is frame_xpl. All the files associated with this analysis will have this jobname as their identifier, which allows them to be recognized easily.

The analysis will run interactively, and messages similar to the following will appear on your screen:

ABAQUS JOB frame_xpl
Begin Analysis Input File Processor
11/11/2004 11:20:05 AM
Run pre.exe
ABAQUS License Manager checked out the following licenses:
ABAQUS/Explicit checked out 5 tokens.
11/11/2004 11:20:09 AM
End Analysis Input File Processor
Begin ABAQUS/Explicit Packager
11/11/2004 11:20:09 AM
Run package.exe
ABAQUS License Manager checked out the following licenses:
ABAQUS/Explicit checked out 5 tokens.
 .
 .
 .
11/11/2004 11:20:12 AM
End ABAQUS/Explicit Packager
Begin ABAQUS/Explicit Analysis
11/11/2004 11:20:12 AM
Run explicit.exe
ABAQUS License Manager checked out the following licenses:
ABAQUS/Explicit checked out 5 tokens.
 .
 .
 .
11/11/2004 11:20:14 AM
End ABAQUS/Explicit Analysis
ABAQUS JOB frame_xpl COMPLETED

When the datacheck analysis is complete, you will find that a number of additional files have been created by ABAQUS. If any errors are encountered during the datacheck analysis, messages will be written to the data file, frame_xpl.dat. This data file is a text file that can be viewed in an editor or printed. Part of this data file is shown in Figure 2–9 through Figure 2–12.

Figure 2–9 ABAQUS input file echo and list of options processed.

Figure 2–10 Model data in data file.

Figure 2–11 History data in data file.

Figure 2–12 Summary of problem and file sizes.

Try viewing the data file in a text editor. The file can contain lines up to 256 characters long, so the editor should be able to accommodate that many characters. At the top of the file is a header page that contains information about the version of ABAQUS used to run the analysis. The header page also contains the phone number, address, and contact information of your local ABAQUS office or representative who can offer technical support and advice.

Following this header page is an echo of the input file (Figure 2–9). The input data echo is generated by adding the option *PREPRINT, ECHO=YES to the input file. By default, the parameter ECHO is set to NO.

Following the input data echo is a list of the options processed by ABAQUS (Figure 2–9). This is the first point at which error and warning messages appear. All error messages are prefixed with ***ERROR, while warnings begin with ***WARNING. Since these messages always begin the same way, searching the data file for warning and error messages is straightforward. When the error is a syntax problem (i.e., when ABAQUS cannot understand the input), the error message is followed by the line from the input file that is causing the error.

The rest of the data file is a series of tables containing all of the model data (Figure 2–10) and the history data (Figure 2–11) that should be checked for any obvious errors or omissions. These tables are generated by including the option *PREPRINT, MODEL=YES, HISTORY=YES in the input file. However, these tables may take up a large amount of disk space for large models. By default, the parameters MODEL and HISTORY are set to NO. You should always check your model by setting MODEL=YES and HISTORY=YES to make sure that what was in the input file was interpreted by ABAQUS in the way you intended. Once you have confirmed that you have the correct input data, you can reduce or suppress this printout if necessary.

Any warning or error messages are written to the data file, frame_xpl.dat, or written to your screen during an interactive analysis. If you submit an analysis without the interactive option, analysis warnings and errors are written to the status file, frame_xpl.sta.

Finally, there is a summary of the size of the numerical model (see Figure 2–12). The comment at the end of the data file that states AN OUTPUT DATABASE REQUEST THAT REQUIRES THE CALCULATOR HAS BEEN FOUND indicates that some of the requested output needs to be converted prior to postprocessing with ABAQUS/Viewer. The types of output that require such conversion using the postprocessing calculator are discussed in “The postprocessing calculator,” Section 4.3.1 of the ABAQUS Analysis User's Manual.