×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

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

Jobs

Abaqus/Python - Extracting Connectivity of Surface Elements

Abaqus/Python - Extracting Connectivity of Surface Elements

Abaqus/Python - Extracting Connectivity of Surface Elements

(OP)
Is there capability within the Abaqus/Python API to extract the connectivity of a surface (such that the element definitions are 2D) from an ODB file? I have only been able to accomplish extracting the 3D elements which are used to form a surface, but I am only interested in the faces.

RE: Abaqus/Python - Extracting Connectivity of Surface Elements

I think there is no direct way to get that info.

Simple workaround (when using A/CAE):
- Create a skin in the property module
- Create a surface section in property module and assign that to skin
- Assign surface element type in mesh module to skin

After the analysis you can take the connectivity of the surface elements.

RE: Abaqus/Python - Extracting Connectivity of Surface Elements

I have done it manually with python by using the surface.elements connectivity, then screening out the nodes that aren't in surface.nodes.

This won't guarantee that the final numbering is in any particular order that would correspond to a 2D element though.

RE: Abaqus/Python - Extracting Connectivity of Surface Elements

When you just have a surface definition (not element), then you get the underlying solid, which is not what you want. Use dummy surface elements as described, place them in a set (named 'skin', e.g.) and then look at the elements of that set. They will output a connectivity with a specific order, which builds the normal direction of that element.

Example:
print session.odbs['Job-1.odb'].rootAssembly.elementSets['SKIN'].elements[0][0]

RE: Abaqus/Python - Extracting Connectivity of Surface Elements

I agree Mustaine that is a better approach. I was just giving an option in case OP didn't want to re-run the analysis :)

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!


Resources