Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Abaqus script issue

Abaqus script issue

Abaqus script issue

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:
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!

RE: Abaqus script issue

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

RE: Abaqus script issue

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.

RE: Abaqus script issue

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

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.


RE: Abaqus script issue

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


Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members! Already a Member? Login


eBook - Integrating the Engineering Ecosystem
Aras Innovator provides multiple options for integrating data between systems, depending on the scenario. Utilizing the right approach to meet specific business requirements is vital. These needs range from authoring tools, federating data from various and dissimilar databases, and triggering processes and workflows. Download Now
Research Report - Simulation-Driven Design for SOLIDWORKS Users
In this engineering.com research report, we discuss the rising role of simulation and the paradigm shift commonly called the democratization of simulation. In particular, we focus on how SOLIDWORKS users can take advantage of simulation-driven design through two analysis tools: SOLIDWORKS Simulation and 3DEXPERIENCE WORKS. Download Now
White Paper - Industry 4.0 and the Future of Engineering Education
With industries becoming more automated, more tech-driven and more complex, engineers need to keep their skills and knowledge up to date in order to stay on top of this wave—and to be prepared for the Industry 4.0 future. The University of Cincinnati offers two online Master of Engineering degree programs designed specifically for practicing engineers. Download Now
eBook - The Design Gridlock Manifesto
In this eBook, you’ll learn 6 ways old CAD technology slows your company down and hear how design teams have put those problems to rest. “The Design Gridlock Manifesto” shares first-hand modern CAD experiences from 15 companies around the world. Download Now

Close Box

Join Eng-Tips® Today!

Join your peers on the Internet's largest technical engineering professional community.
It's easy to join and it's free.

Here's Why Members Love Eng-Tips Forums:

Register now while it's still free!

Already a member? Close this window and log in.

Join Us             Close