Extraction of Stresses with Python at each integration points 1

[Jeje3103]

online
1 post
This post has NOT been accepted by the mailing list yet.
I m trying to extract the stresses with Python at each integration points (or an extrapolation to the nodes). I get the stresses but i dont succeed to use a nodelabel or something like that to
know where i m extracting data...
My aim is to extract some values as plastic strain and re use it in an other calculation so i
need to know exactly the labelling

My code is :

from odbAccess import *
import numpy as np

odb = openOdb(path='C:/Users/Jerome/Desktop/test_couplageFEM_DIC/Fish.odb')

lastFrame = odb.steps['Step-1'].frames[-1]

stress=lastFrame.fieldOutputs['S']
sortie = open('Resu_PE_maillage.txt', 'w')
sortie.write('Node label \t S11 \t\t S22 \t\t S33 \t\t S12 \t\t S23 \t\t S13 \n')

for S in stress.values:

sortie.write('%.10e\t\t %.10e\t\t %.10e\t\t %.10e\t\t %.10e\t\t %.10e\n' % (S.data[0], S.data[1], S.data[2], S.data[3], S.data[4], S.data[5]))

sortie.close()

 

[Mustaine3]

Integration Points are not related to nodes, they are related to elements. Within an element they are numbered.

Check the "Report" option in /CAE postprocessing. Here you can export these results to an ASCII file.

The location of the integration points can be requested as output with
*Element Output, Position=Integration Points
COORD

 

[Jeje3103]

Thanks for your help!
But i would like to optimize this obtainement because i would re use some results as plastic strains in further
computations

 

[Mustaine3]

What exactly is your question now?

You could easily extract the extrapolated (but unaveraged) values at nodes. Just request them for the analysis to get them written in the ODB.
*Element Output, Position=Nodes
S

 

[Jeje3103]

Sorry i dont understand...i have to request that where in abaqus?
I have 6.13 Abaqus and i m looking for in the "Edit Field Output Request"
or i have to add that in my inp file?
Thanks for your help

 

[Mustaine3]

That's not supported in /CAE. You have to add that into the input file or maybe the /CAE Keyword Editor.

 

[Mustaine3]

But again, there is no averaging happening, so you have multiple stresses at one node.
Averaging is done during graphical postprocessing. A report could write these values in a file.

 

[Jeje3103]

Ok thanks!

So at the end of my .inp file, i have to add "*Element Output, Position=Nodes" in field output?

** OUTPUT REQUESTS
**
*Restart, write, frequency=0
**
** FIELD OUTPUT: F-Output-1
**
*Output, field, variable=PRESELECT

**
** HISTORY OUTPUT: H-Output-1
**
*Output, history, variable=PRESELECT
*End Step

 

[Mustaine3]

This keyword cannot exist standalone. You have to indicate that this request is for the ODB and that it is field output. So it should look like this:

*Output, field
*Element Output, Position=Nodes
S

You can modify that depending on the variables you would like to have or the output frequency.

See Abaqus Users Manual 4.1.3 Output to the output database