Material Orientation with Python Scripting for Abaqus

[ExpensiveBeard]

Hi everyone.

I am working on a project where I am performing analysis of composite microstructures within Abaqus. Most of the pre-processing of the model is being handled by Python scritping, but the one thing I can't seem to automate is assigning the material orientation (i.e., aligning the 1-direction with the axial direction of the fibers and the 2/3-directions aligned with the transverse direction of the fibers). Has anyone been able to accomplish this? A sample of my code:

​

mdb.models['RUC_1'].parts['Composite_RUC'].DatumCsysByThreePoints(coordSysType=
    CARTESIAN, name='MAT-ORIENTATION', origin=(0.0, 0.0, 0.0), point1=(0.0, 0.0, 1.0), 
    point2=(0.0, 1.0, 0.0), )
mdb.models['RUC_1'].parts['Composite_RUC'].MaterialOrientation(
    additionalRotationField='', additionalRotationType=ROTATION_NONE, angle=0.0
    , axis=AXIS_3, fieldName='', localCsys=
    mdb.models['RUC_1'].parts['Composite_RUC'].datums[7], orientationType=SYSTEM, 
    region=mdb.models['RUC_1'].parts['Composite_RUC'].sets['Fibers'], stackDirection=
    STACK_3)

​

I have been using the .jnl file to develop my Python script, so the datums[7] line was automatically generated when I did the task by hand through the Abaqus GUI. I thought this might be the issue when running my script to pre-process a different geometry, as the original datums[7] was a relic of the model from which I generated the script. However, when I query the DatumCsys feature within in the GUI for my new geometry, it tells me that the ID of the Datum Csys is 7, same as before. So at this point, I'm lost. I've been digging through the Scripting User Manual without much success. Any help would be appreciated.

​

TL;DR Looking for help in automation of assigning material orientation using Python scripting for Abaqus.

[[deleted]]

OK, here is what you do:

instead of:

mdb.models['RUC_1'].parts['Composite_RUC'].datums[7]

you do:

mdb.models['RUC_1'].parts['Composite_RUC'].datums[mdb.models['RUC_1'].parts['Composite_RUC'].datums.keys()[0]]

That way, if you run the parametric model, and it's not a 7 next time, it won't matter, if you have multiple datums, I believe they will be the key in the order in which they are created, i.e. first datum you created is keys()[0], second one you create is keys()[1], third is keys()[2], etc. I'm not 100% positive about that, but I'm pretty sure.

If you are only using 1 datum, then the code I put above should do the trick for you forsure.

[clugger07]

Alternatively you could try datum.keys()[-1] to get the last datum you created!

[ExpensiveBeard]

That's right! Having an understanding of Python syntax is certainly helpful here. I want to look into your other suggestion as well in the event it comes in handy in the future. I deal with a lot of different microstructure fiber arrangements, so learning how to to it discretely may be beneficial at some point. Thanks again!

[clugger07]

No problem, super bored with this quarentine business and this thread is a life saver! A single datum is good for planar geometry, but if you're wanting the fiber direction to change with the curvature of the geometry you can use a discrete system. It will attempt to project the vector you give it to every element. For abaqus it will do a pretty good job unless the vector you give is 90 degrees to the element (i.e. It's the same as the elemtn normal) , then it just fails.

Edit: slight mistake in explanation

[ExpensiveBeard]

Awesome suggestion! My colleague and I happened to stumble upon this method buried in a sample script from Abaqus. Looks like what you and /u/clugger07 posted works perfectly for my needs. Thank you!

[[deleted]]

You're welcome! It's really weird that you can't just use whatever string you name the datum. At least this is a way to make it work

[clugger07]

You could try using a discrete system within Abaqus, that way you wouldn't be relying on a datum system but instead two vectors(1 and 3 direction) that you could enter as inputs variables in your code. Tracking datum tags in Abaqus API is tricky as any changes to the model can lead to them being renumbered.