Abaqus script issue

[schopenhauer]

Hello everybody,

I have been doing so many simulations for pipes lately that I decided to create a very simple plugin for Abaqus to create 1/4 section models. I didn't have any experience or knowledge building scripts for Abaqus but with the manual, the *.rpy file and a bit of imagination I got what I wanted. But, something is failing that I'm not able to solve. When I want to submit the job, the following error message appears:

The region selected for the following loads contains invalid geometry or mesh components for the load type. Pressure.

I suspect that this is related with the definition of the load in the script:
#Pressure
inner_face_center = (Ri/2,(Ri**2-(Ri/2)**2)**.5, pipe_length/2)
inner_face = myInstance.faces.findAt((inner_face_center,) )
pressureRegion = (inner_face,)
myModel.Pressure(name='Pressure', createStepName='Load_step', region=pressureRegion, magnitude=Pi)

But it is weird because I used the same technique to apply the boundary conditions without any problems:
#z symmetry
left_side_center = ((Ri+Ro)/2,1,0)
right_side_center = ((Ri+Ro)/2,1,pipe_length)
left_face = myInstance.faces.findAt((left_side_center,) )
right_face = myInstance.faces.findAt((right_side_center,) )
Zsym_region = (left_face, right_face)
myModel.ZsymmBC(name='BC-1', createStepName='Initial', region=Zsym_region, localCsys=None)
#x symmetry
xxx_side_center = (0,(Ri+Ro)/2, pipe_length/2)
xxx_face = myInstance.faces.findAt((xxx_side_center,) )
Xsym_region = (xxx_face,)
myModel.XsymmBC(name='BC-2', createStepName='Initial', region=Xsym_region, localCsys=None)
#y symmetry
yyy_side_center = ((Ri+Ro)/2, 0, pipe_length/2)
yyy_face = myInstance.faces.findAt((yyy_side_center,) )
Ysym_region = (yyy_face,)
myModel.YsymmBC(name='BC-3', createStepName='Initial', region=Ysym_region, localCsys=None)

Finally, by editing the step and selecting the same surface, the analysis is able to run. Any ideas what is happening with the code?

Many thanks!

 

[FEA way]

I think that this is because you should use Surface type object for pressure definition.

 

[Mustaine3]

Correct. A surface is not the same as a face. A surface contains an information about a direction, which is needed for contact or a pressure load.
A face used in a boundary conditions is finally nothing else than it's nodes. There is no direction needed.

Apply a pressure load in the GUI and look in the .rpy what the commands are.

 

[schopenhauer]

FEA way, Mustaine3, thank you very much for your quick answers.

Indeed, the problem was the surface definition, a different method had to be used. If you use the *.rpy command starightaway, you will get the following command:

side1Faces1 = s1.getSequenceFromMask(mask=('[#4 ]', ), )

Which is not very useful, you first need to pass the line

session.journalOptions.setValues(replayGeometry=COORDINATE, recoverGeometry=COORDINATE)

into Abaqus, to get the more useful

side1Faces1 = s1.findAt(((39.914602, 2.612383, 66.666667), )).

All together, the pressure definition is done by

#Pressure
s1 = myAssembly.instances[part_name].faces
inner_face = s1.findAt(((Ri/2,(Ri**2-(Ri/2)**2)**.5, pipe_length/2), ))
pressureRegion = regionToolset.Region(side1Faces=inner_face)
myModel.Pressure(name='Pressure', createStepName='Load_step', region=pressureRegion, magnitude=Pi)

I hope this helps others with similar problems. And again, I'm very grateful for all the help received.

Cheers!

 

[Mustaine3]

You can change the way A/CAE reports the selected geometry. Enter this in the A/CAE CLI to switch the method.

session.journalOptions.replayGeometry
session.journalOptions.setValues(replayGeometry=INDEX)