How to read averaged nodal stress from abaqus odb file using python script?

Question

I know how to read element or element node stress value (unaveraged) using python script.

field = stressField.getSubset(region=topCenter,position=INTEGRATION_POINT, elementType = 'CAX4')

But i want averaged stress values at nodes. FYI, my odb does not contain node position data for stress (i.e., position=NODAL).

Answer 1

this is one of those things that way more cumbersome than it should be. you need to create xydata :

session.xyDataListFromField(odb=odb,
        outputPosition=ELEMENT_NODAL,
        variable=(( 'S', INTEGRATION_POINT), ),
        elementSets=('PART-1-1.SETNAME', ))

this creates a dictionary with objects for every node of every element and every stress component (ie. huge). Unfortunately the dictionary is keyed by cumbersome descriptor strings, eg:

 session.xyDataObjects['S:S11 PI:PART-1-1 E: 15 N:2'].data

gives the 11 stress component of node 2 associated with element 15. To make use of the data in a script you need to either construct the strings, or loop over the dictionary and parse the positionDescription for each object.

Edit: if you want the nodal averages its pretty much the same. You do:

session.xyDataListFromField(odb=odb,
        outputPosition=NODAL,
        variable=(( 'S', INTEGRATION_POINT), ),
        nodeSets=('PART-1-1.SETNAME', ))

and the dictionary objects are keyed like:

 session.xyDataObjects['S:S11 (Avg: 75%) PI:PART-1-1 N:2'].data

note you can issue multiple session.xyDataListFromField calls and all of the data goes into xyDataObjects (For example if you want stress and strain you can process both at once. )

For completeness, if you only want a specific component(s) you can request as:

 variable=(( 'S', INTEGRATION_POINT,((COMPONENT, 'S11'),)), )