How to use Abaqus2Matlab with Abaqus/Explicit studies?
Thank you very much for your interest in Abaqus2Matlab.
Regarding your issue, please replace the option *FILE FORMAT, ASCII with the option *FILE OUTPUT in the input file (.inp). The former option works only for Abaqus/Standard whereas the latter only for Abaqus/Explicit.
Do not forget to specify at least one of the following options after *FILE OUTPUT:
*CONTACT FILE *EL FILE *ENERGY FILE *MODAL FILE *NODE FILE *SECTION FILE
The above options in an Abaqus/Explicit analysis define the output to be written to the selected results file. After running the input file in which the above options are specified, a selected results file in binary format will be created, with the extension *.fil.
After this, you have to convert this file from binary format to ascii format. You can do this by executing in the Abaqus/Command window the following statement:
abaqus ascfil job=[filename]
where [filename] is the name of the file [filename].fil that is generated after the Abaqus/Explicit analysis has run. The last command will generate a new results file in ascii format, named [filename].fin. You can postprocess this file to obtain the results that you want in Matlab in the classic way, i.e. first obtaining its contents to an one-row string (using the function Fil2str.m) and afterwards reading the desired results by using the proper RecXXX.m function (look in the file Documentation.pdf for more information).
With a view to being as friendly to the user as possible, Abaqus2Matlab has documented one verification example for each different postprocessing function. The verification examples can be found in the "Verification" folder of the toolbox. You can find many examples that illustrate the use of functions RecXXX.m, named as VerifyXXX.m. In each of these functions, the postprocessing procedure is implemented in a way easily comprehensible by the user. You can copy any of these examples and use it as a template to adjust it to fit your own post-processing task.
Please, find in this link an example input file of an Abaqus/Explicit analysis retrieved from the Abaqus Documentation, named 1.inp. This input file concerns a composite shell in cylindrical bending.
The steps to be followed to obtain the results of this analysis are the following:
1) Execute in the Abaqus/Command window abaqus job=1 to run the Abaqus/Explicit analysis. After the analysis terminates, the selected results file is created (1.sel)
2) Execute in the Abaqus/Command window abaqus job=1 convert=select to convert the selected results file into a results file, i.e. convert 1.sel to 1.fil.
3) Execute in the Abaqus/Command window abaqus ascfil job=1 to convert the results file in binary format to the same results file to ascii format, i.e. convert 1.fil to 1.fin.
4) Apply Abaqus2Matlab to retriene the desired results from the file 1.fin.
I hope this will help you. In case that your problem remains, do not hesitate to ask for more details and/or recommendations from the Abaqus2Matlab work team.
Good luck and success with your Abaqus2Matlab experience.
Enjoy the novel way of postprocessing Abaqus output.
Use Abaqus2Matlab, the alternative choice.
With best regards,
George Papazafeiropoulos (Abaqus2Matlab work team)