request fieldouput about node stress

[cclcjp228]

Hi all,

I am trying to extract nodal stress (shear stress) from odb file using a python script.
I first defined a field request in CAE with a domain of a set of nodes, which in INP file is shown as "*Output, field *Node Output, nset=Set-1, variable=PRESELECT". and i select stress to be the requested varible.
the part of my script is:
Nodeset = odb.rootAssembly.nodeSets['SET-1']
ReactionForce = frame.fieldOutputs['S'] # this certain frame has been previously defined.
ReactionForceInterest = ReactionForce.getSubset(region=Nodeset).values

however, i get zero values from above script.
Can someone suggest? thanks in advance.
Hoping to hear from some one soon.

Cheers

 

[Mustaine3]

Stresses are still element output, even when you request that Abaqus extrapolates the values to the nodes. So you have to use an element set (or nothing) and
*Element Output, Position=...

See Keyword Reference Manual for the details.
This keyword option is not supported through /CAE, so you have to add manually it into the input file or the CAE keyword editor.


And be aware, that prior v2016 the values can only be extrapolated by the solver, but not averaged.

 

[cclcjp228]

Dear Mustaine3,

thanks for your reply. just to confirm, so did you mean there is no direct method to extract the nodal stress?
and my second question is:
i had succeeded to extract the elemental stress. based on my understanding, is it right that the only way to get 'true' nodal stress would be averaging the nodal stress (i.e. the stress on the corners of each element) of every element that shares that node?

thanks again

 

[Mustaine3]

Extrapolation and averaging is usually a task of the postprocessing tool. Maybe you don't try reading the ODB directly, but automate that A/CAE as postprocessor opens the ODB and writes an report with the stresses at the nodes. There you'll find what you're looking for.

 

[cclcjp228]

Dear Mustaine3,

thanks again for your reply. i actually need to extract shear stress related customised variable: shear stress* displacement, over every frame.
i am sure that can be done through CAE by exporting each variable and multiplying together, which also can be very time and labour consuming.
So, is that the only method that i can do?

thank you again.

 

[Mustaine3]

I see two options for your process:

1. Without postprocessing tool:
- request stresses extrapolated to nodes from solver
- with script:
---- read stresses at nodes
---- do averaging
---- read displacements
---- calculate your result
---- repeat for next frames

2. With postprocessing tool:
With script:
- open regular odb in /CAE
- create report with displacement and stresses at nodes for first frame
- read data from report
- calculate your result
- repeat last three actions for other frames