Python Scripting - for element info 1

[macroguy]

For the ABAQUS Experts out there,

I have written a small pyhton script that loops through all the elements in the model and writes out the nodal coordinates & element connectivity for each element. However I am not able to get the material number assigned to each element.

What scripting commands should I be using to query for the material number associated with each element? I would really appreciate it if someone out there can let me know how to do this.

regards
BV

 

[xerf]

You obtain the material via the section object.

Thus, you need to extract the name of the section.

Then:
from model:

model=mdb.models['My model name']
section=model.sections['Section name']
material=model.materials[section.material]

from odb:

import odbMaterial
import odbSection


odb=session.odbs['my odb']
section=odb.sections['Section name']
material=odb.materials[section.material]

For the odb case you need to obtain first the section assignment object.

Each odbInstance in the assembly has a sequence of
section assignments:
instance=odb.rootAssembly.instances['my odbInstance']
assignments=instance.sectionAssignments

each section assignment has 2 attributes:
set_i=assignments.region -> an OdbSet object
section_i=assignments.section -> a Section object

the OdbSet has an array of elements which you can be iterated (i.e. set_i.elements)

 

[macroguy]

xerf,

thanks for the insightful reply. I have few questions however.

1. I am not using the odb to get this information, all i am doing is using ABAQUS as a pre-processor to get my mesh information, which I am writing out to a seperate file and solve it uisng a coustom code. So, instead of using
" instance=odb.rootAssembly.instances['my odbInstance']"

can i use

"instance= mdb.models['my model'].rootAssembly.instances".

2. By using mdb instances, will there still be 2 attributes you described for each section assignment, and what should I be looking for instead of the 'odbSet'.

3. Fianlly, where can I find all this information? I have looked up the ABAQUS scripting documentation online and couldnt find what you told me. I would be grateful to you if you can point me to some extensive source I can look up before posting my questions online.

regards
BV

 

[xerf]

1.instance= mdb.models['my model'].rootAssembly.instances['instance name']

2.odbSet is an object (class) associated with the .odb output database file, therefore if you are using CAE only as pre-processor you do no need odbSet.

In ABAQUS Scripting Interface (ASI) there are two main classes:
(i) mdb storing the pre-processing info
(ii) odb storing the post-processing info

Any class having its name starting with "odb" relates to the output database and to an odb object.

If you are using CAE only as a pre-processor and you are not convenient with the architecture of the ABAQUS Scripting Interface (ASI), a simpler approach would be to write the input file and extract the information from the input file (.inp) which is a text file.

CAE->Job module->Job Manager ->Write input.

The input file should be very easy to parse (especially if you are using Python) and it is prety much self-explanatory.

3. For ABAQUS Scripting Interface I use only "Scripting Reference Manual". To become convenient with the ASI structure , I think, one should start with the "Scripting User's Manual".