×
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

Meshing of a complex geometry tissue in Abaqus

Meshing of a complex geometry tissue in Abaqus

Meshing of a complex geometry tissue in Abaqus

(OP)
Hi everyone,

I am trying to do a finite element analysis of the Temporomandibular joint disc (TMJ disc) in Abaqus. I already got the IGES model of disc from Hypermesh but the geometry needs so much partitioning to become suitable for at least Tetrahedral mesh. Would you please tell me if the partitioning is the only way and if it is the what would be the best way to do it?

I think there should be easier method to do it since I have sen much more complex geometries (like brain tissue) which has been meshed by Abaqus. I would appreciate if anyone can help me.

RE: Meshing of a complex geometry tissue in Abaqus

Do yourself a favor, don't bother making these geometries using MRI/CT scans; just make realistic but simple geometries using SolidWorks. Use boundary or loft feature to make a 3D model and export it as an .SAT or as a .STEP file which can be easily imported into ABAQUS and meshed in seconds.

http://www.eng-tips.com/faqs.cfm?fid=376

RE: Meshing of a complex geometry tissue in Abaqus

Another option is to smoothen the geometry as best as you can. Geomagics is pretty good at it and MIMICS and Simpleware have functions to accomplish that. Also, freely available Slicer3D may also have these options. Finally, another freely available and user friendly software called IAFeMesh may get you a hex mesh for this geometry.

http://www.eng-tips.com/faqs.cfm?fid=376

RE: Meshing of a complex geometry tissue in Abaqus

(OP)
Thanks for your quick responses. Actually the real geometry of this tissue is of high importance due to its thickness variation along the anteroposterior and mediolateral directions. On the other hand, According to literature,recently, they have been using MRI/CT even more than before. I am also planning to consider collagen fibers in the analysis which makes it totally important to have the most realistic geometry.

I am just wondering if this is the normal way of meshing such a complex geometry and if the answer is yes, then how they do meshing on much much more complex geometries in Abaqus? Don't you think it's better to do the meshing in Hypermesh (which I think is a better software for meshing although I am not sure if it also needs partitioning or not) and then import the model including mesh to Abaqus as a .inp file?

Btw, @IRstuff: I am not sure what you mean by decimating it, but i want to run an analysis on the whole model.

I appreciate your helps.

RE: Meshing of a complex geometry tissue in Abaqus

One can make "realistic" 3D models of cervical vertebrae - which are far more complicated than discs - using SolidWorks. TMJ is no big deal.

http://www.eng-tips.com/faqs.cfm?fid=376

RE: Meshing of a complex geometry tissue in Abaqus

(OP)
@IceBreakerSours: you're definitely right, Abaqus is not a good solid modeling software. I used to work with Solidworks and it's quiet more user friendly in terms of making solid models. At the moment, the University doesn't support Solidwork, otherwise I would import 2D image stacks of tissue into it and make a 3D reconstruction which could easily be meshed.

Btw regarding the meshing software you mentioned above, do you mean I can do the meshing there and then import it to Abaqus? Is the meshing procedure different from Abaqus (doesn't need partitioning)? because I know on of my friend used Hypermesh to mesh the model with Tetrahedral element and he said the software did it automatically although the mesh quality might be not that good. Then he imported the meshed model into abaqus and did the rest.

@rstupplebeen: I've tried working with Virtual topology which makes it smoother as you said but I was wondering if the partitioning is the only method to do mesh such a geometry.

Tnx

RE: Meshing of a complex geometry tissue in Abaqus

Yes, almost every program I mentioned previously provides an output format that ABAQUS can import. I am not sure about Slicer3D.

Also, try to zoom in into the geometry and check for some small features like edges. You must ignore those features using virtual topology. Finally, quadratic elements can conform to curved geometries but before you use quadratic elements, make sure the geometry is free of any issues. Note that quadratic elements are not recommended for contact (unless they are modified).

http://www.eng-tips.com/faqs.cfm?fid=376

RE: Meshing of a complex geometry tissue in Abaqus

(OP)
And I have another question regarding making a fiber-reinforced model. the collagen fiber can be modeled as fibers inside the tissue. Basically, there are two main methods to model fiber reinforced materials , one is to use spring btw the nodes which makes the fiber directions limited to node distances and the other one is to use continuum model and define two separate material for the fibers and the medium surrounding the fibers including the interaction btw them.

Since I am new to abaqus, I don't know from where to start. Do I have to simply make holes inside my models and pass tube shape fibers through them and then define a material for them? in which step should I use the spring between the nodes? What is the SPRINGA element? I found all these keywords while i was searching but I still haven't managed to implement any technique yet. I would appreciate if anyone can give me a clear framework, and ideally, an step by step procedure although i know it's different case to case and you might need to know more details.

RE: Meshing of a complex geometry tissue in Abaqus

Use the Holzapfel material model. Up to 3 fiber directions (anisotropy, to be accurate) can be incorporated. In the Holzapfel model, fibers don't take load under compression (ground substance does). See the Abaqus documentation for details.

http://www.eng-tips.com/faqs.cfm?fid=376

RE: Meshing of a complex geometry tissue in Abaqus

Use Hypermesh if you have it. You can check and correct mesh quaility and even downsample if you need to.

We use Hypermesh or Amira and dont really touch Abaqus CAE until the last step of setting the model up. Simpleware is also really good especially for setting up contact surfaces.

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