This chapter illustrates how to write and utilize postprocessing programs to manipulate data stored in the ABAQUS results file. The results file, which is identified by the file extension .fil, is created by the *CONTACT FILE, *EL FILE, *NODE FILE, *ENERGY FILE, *MODAL FILE, and *RADIATION FILE options and contains results based on user-specified output requests. The standard file format is binary, but it can be changed by user request for each run with the *FILE FORMAT, ASCII option. 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 “Execution procedure for making user-defined executables and subroutines,” Section 3.2.13 of the ABAQUS Analysis User's Manual). 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 Chapter 5, “File Output Format,” of the ABAQUS Analysis User's Manual 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 Chapter 8, “Using the ABAQUS Scripting Interface to access an output database,” of the ABAQUS Scripting User's Manual or Chapter 9, “Using C++ to access an output database,” of the ABAQUS Scripting User's Manual for information on accessing data stored in the ABAQUS output database.
Details about the variables that are used in the postprocessing programs are discussed in “Accessing the results file information,” Section 5.1.3 of the ABAQUS Analysis User's Manual. 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,” Section 5.1.3 of the ABAQUS Analysis User's Manual, 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 manipulation requires knowledge of each data record. Details of these records are found in “Results file output format,” Section 5.1.2 of the ABAQUS Analysis User's Manual.
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,” Section 5.1.4 of the ABAQUS Analysis User's Manual.