×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

Extraction of Stresses with Python at each integration points

Extraction of Stresses with Python at each integration points

Extraction of Stresses with Python at each integration points

(OP)
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()

RE: Extraction of Stresses with Python at each integration points

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

RE: Extraction of Stresses with Python at each integration points

(OP)
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

RE: Extraction of Stresses with Python at each integration points

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

RE: Extraction of Stresses with Python at each integration points

(OP)
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

RE: Extraction of Stresses with Python at each integration points

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

RE: Extraction of Stresses with Python at each integration points

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.

RE: Extraction of Stresses with Python at each integration points

(OP)
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

RE: Extraction of Stresses with Python at each integration points

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

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources