Exporting ABAQUS output results 1

[Ingeniosus]

Hi everyone!
I'm trying to export ABAQUS results of a fem analysis in a file format like .txt or equivalent.
Is it possible?
I only had a .fil file, but it's very incomprehensible and I will need a MATLAB code to interpret every single code.

Thank you

 

[RBillard]

Hi,
Yes you can. Extract the data you need. Then in the menu bar, select "report", "xy", and saves the data to a file ".rpt" which is silimar to a file ".txt"

 

[Ingeniosus]

Thank you very much!
It works!!

 

[tetmesh]

Is there a way to do this with an Abaqus/Explicit job that doesn't require clicking through the 'Output Databases' tree to save pre-requested history outputs as XY data? I'd like to see the xy data from my history outputs without opening CAE.
Thanks you.

 

[Ingeniosus]

I know that you can export directly an output file through modifying code in the input file. You can do this on the menu bar EDIT KEYWORDS.
You have to write after HISTORY OUTPUT (for exemple to export displacement U):

* NODE SET, set=yoursetname, frequency = 1
U

I tried this and ABAQUS create in your work directory a ".fil" file with all results you need but it is very incomprehensible ad you will need a FORTRAN program or a MATLAB program to separate ad interpret all codes.

 

[RBillard]

You must create a macro, it is to save the extraction step results only once. You can then run this macro and recover your data without opening ABAQUS CAE, using this command for example:


"abq69ef1 cae noGUI=D:\documents\Abaqusmacro.py"


Here are all the steps before you can run the macro with the command:

1)Submitt jour job in ABAQUS CAE
2)When the calculation is complete, close ABAQUS CAE
3)Open ABAQUS CAE
4)Click on "file" then "Macro Manager" in the menu bar, "create","continue"

Now, you are currently recording everything you do.

5) open your job.odb
6) extract your results
7) select "report", "XY", Save your data in a rpt file.
8) Now, you can stop the recording of the macro.

Now you are going to test your macro. Close Abaqus CAE and open it again.

9) Click on "file" then "Abaqus PDE" in the menu bar, and open your macro.
10) Remove the line: "def macro():" Run it,If you have errors, removes spaces before each line in the macro and run it again.


If the execution of the macro works, and you have well auto-generate the rpt file. You can close ABAQUS CAE and execute the command:

abq69ef1 cae noGUI=D:\documents\Abaqusmacro.py
(with the correct version of ABAQUS and the correct path to your macro)

 

[Ingeniosus]

I found this command to force ABAQUS creating a .DAT output file with all node variables:

**
** FILED OUTPUT: H-Output-1
**
*Output, history, variable=PRESELECT
*NODE PRINT, nset=yourNameSet
COORD, NT

You have to write it in the INPUT FILE (MODEL --> EDIT KEYWORDS) just before the *end.

I found also this one to print stress and displacement:

*NODE PRINT
U,
RF,
*EL PRINT
S,

But is there a way to have an output .DAT file with a single table for all TIME STEPS and with all variables??

Thank you