Sukirti Dhital Script execution

1. At the system prompt, type abaqus python scriptname.py. The following statement must be included in the script: import from odbAccess *

2. Select FileRun Script from the Abaqus/CAE main menu bar, and then browse to the file you want to run. The following statement must be included in the script: import from visualization *

Take a look at this as well: https://www.eng-tips.com/viewthread.cfm?qid=452095

Qamar Ul Islam Thank you for the response. This method would work if I generate odb file and have a template mesh size. But is it possible to determine element center coordinates in the preprocessing script, after sketching the part and generating the mesh? I figured out "elements.label" command gives each element label. I tried using getCoordinate(label) to get the element center but I believe this is not the right command. Abaqus user manual too could not guide me in the right direction.

The only method that I have figured out is to get nodes of each element using getnodes() command and then average the nodes to get the element center. But I believe this will be computationally expensive for a very large model. If anyone has a better idea please suggest.

Dear Sukirti,

to get directly the element centroid you can loop through your elements and request the Mass properties of it specifying the "volumeCentroid".

a = mdb.models['Model-1'].rootAssembly

elements1 = element/selection of elements

a.getMassProperties(regions=elements)["volumeCentroid"]

elements1 must be a region.

I hope it helps.

Hi Federico Danzi ,

Thank you for the suggestion. Can I create a region for a single element? When I tried, on my end, it seems like a region can only be created for a sequence of tuples indicating vertices, edges, faces or cells. Since in my case I have a single face, that has been meshed, and based on coordinates of each meshed element, I develop a set which are then assigned material property. Unfortunately I could not select each element to form a region and loop it to check the coordinates.

Regards,

Sukirti

Hi Sukirti,

I have been a bit vague in the first reply; here are the commands in detail:

import regionToolset

a = mdb.models['Model-1'].rootAssembly

elements = a.instances['Part-1-1'].elements

centroid_list = []

for i, el in enumerate(elements):

print(el)

region = regionToolset.Region(elements=elements[i:i+1])

properties = a.getMassProperties(regions=region)

centroid_list.append(list(properties['volumeCentroid']))

print(centroid_list)

I tried with a unitary cube with 2 elements per edge and it works fine.

I hope it helps.

Hi Federico Danzi ,

I am sorry for the late reply but this worked for me. :)

Thank you for such detailed explanation.

Regards,

Sukirti