About user postprocessing of Abaqus results files

You can write and utilize postprocessing programs to manipulate data stored in the Abaqus results file.

The following topics are discussed:

The Abaqus results file is identified by the file extension .fil and contains results based on user-specified output requests; see Output to the Data and Results Files for more information on the types of data that are written to the results file. The standard file format is binary, but it can be changed to ASCII format for each run by user request. Alternatively, it can be set to a default ASCII format during site installation. Abaqus uses Fortran unit 8 to communicate with the results file.

Sample postprocessing programs that perform commonly exercised tasks are presented in separate sections in this chapter. These include merging multiple results files and converting the resulting results file from binary format to ASCII, or vice-versa; computing principal values and directions of stress and strain; and computing a perturbed mesh for a collapse analysis by incorporating a user-specified geometric imperfection in the form of the critical buckling mode shape.

Each postprocessing program must be linked using the make parameter when running the Abaqus execution procedure (see Making user-defined executables and subroutines). To link properly, the postprocessing program cannot contain a Fortran PROGRAM statement. Instead, the program must begin with a Fortran SUBROUTINE with the name ABQMAIN.

General programming concepts, Abaqus Fortran interfaces, and data processing concepts are described below. Refer to File Output Format for additional information. The program listings in each section provide details on the program flow, how to interface with various computer platforms that use different operating systems and Fortran compilers, and how to interface with Abaqus subroutines to handle data files and records.

Refer to Using the Abaqus Scripting Interface to access an output database or Using C++ to access an output database for information on accessing data stored in the Abaqus output database.

Initialization

Details about the variables that are used in the postprocessing programs are discussed in Accessing the results file information. Abaqus uses a 512-word buffer named ARRAY for the reading and writing of data on the results file. This is dimensioned as ARRAY(513). The integer equivalent is JRRAY(513) for a 64-bit computer or JRRAY(2,513) for a 32-bit computer. The EQUIVALENCE statement is used to equivalence ARRAY and JRRAY to simplify manipulation of real and integer numbers in the data record stored in the buffer.

The information concerning the Fortran unit number and format of the results file that is read is defined in LRUNIT(2,NRU), where NRU is the number of files to be processed. The Fortran unit number for the nth file is stored in LRUNIT(1,n). The information about the file format is stored in LRUNIT(2,n), which is initialized to 1 for ASCII format and to 2 for binary format. If a new results file is to be created by the postprocessing program, the file format of the output file is defined similarly via the variable LOUTF, which is also initialized to 1 for ASCII format and 2 for binary format. The root file name for both input and output results files is defined through the character variable FNAME. The root file name case will be the same as the case in which FNAME is defined; Abaqus defines the file extensions to be lowercase letters. See Accessing the results file information for a discussion of the naming convention for the file extensions.

The final initialization phase is done internally by calling the Abaqus subroutines INITPF and DBRNU. The Fortran interfaces are 

CALL INITPF(FNAME, NRU, LRUNIT, LOUTF)
CALL DBRNU (JUNIT)

where the arguments in the call to INITPF are as described above, and JUNIT is the Fortran unit number connecting the file.

These integer variables must be defined before the subroutines are called.

Data processing

Data manipulation requires knowledge of each data record. Details of these records are found in Results file output format.

The data organization in the results file uses a sequential format. Each record must, therefore, be retrieved in a sequential manner via a call to DBFILE using the interface 

CALL DBFILE(0, ARRAY, JRCD)

This call can be placed inside a DO-loop, and the loop count should exceed the number of records stored in the file. Alternatively, DBFILE can be called as long as JRCD is equal to 0. The first argument, 0, indicates that a record is to be read. Each record that is read is stored in the buffer ARRAY and returned to the calling program for manipulation. The last argument, JRCD, is a return code that is set to 0 unless an end-of-file condition or an incomplete record is processed, in which case JRCD is set to 1.

If it is desirable to extract or modify certain records and save them in a new results file with the same data organization as an Abaqus-generated results file, then the subroutine DBFILW should be called with the interface 

CALL DBFILW(1, ARRAY, JRCD)

The new results file will be written with the file extension .fin. Refer to Utility routines for accessing the results file.