×
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

Help meshing a complex part

Help meshing a complex part

Help meshing a complex part

(OP)
Hi all,

I'm meshing a lattice like solid structure but having nightmare meshing it. Would any kind hearted person have a look at it and help me mesh it? Automatic mesh is not possible, so I used Tet elements but elements are distorted. So best is to get Hex (C3D8) elements.

The cae file (Version 6.14) is here - https://www.dropbox.com/s/jw3mryb50k7kr8d/Mesh_pro...


Thanks!

RE: Help meshing a complex part

I had no problem creating a tet mesh. I used a global mesh seed of 1e-4 and the default curvature control.

RE: Help meshing a complex part

(OP)
I'm using it in a Abaqus/Explicit analysis, element size of ~1e-4 will result in huge computation time. So I need Hex element to achieve optimal performance. Can you please try to create a all Hex mesh?

RE: Help meshing a complex part

(OP)
Tet element results in weeks of computational run time (Abaqus/Explicit), Hex is absolute must. Also, Hex elements are much more robust and preferable.

Anyone? Help please!

RE: Help meshing a complex part

Then maybe your only other option is to change your base units?

As pointed out by people above, who know what they are talking about by the way, the geometry of your structure is better suited to tets.

RE: Help meshing a complex part

Can't you exploit symmetry? If you can not, then why not hex mesh just a replicating "unit" of the part geometry (like one rod/beam in Part module) and arrange the hex mesh in the correct pattern in the Assembly module? At worst, you have may to have move some nodes if you wish to have coincident nodes. Otherwise, a tie constraint will do the job too.

Answers to such questions will be informed by what you wish to accomplish with the model, how you are validating your model, etc.

Are you new to this forum? If so, please read these FAQ:

http://www.eng-tips.com/faqs.cfm?fid=376
http://www.eng-tips.com/faqs.cfm?fid=1083

RE: Help meshing a complex part

(OP)
I have partitioned a single beam and it gives all Hex elements. But problem starts when I try to do it on the whole structure.


Single beam, partitioned to achieve Hex elements -




Single beam, meshed with Hex elements -



Mirrored beam, Magenta colored region is not mesh-able to achieve Hex -




Again, Magenta colored region is not mesh-able to achieve Hex -




So guys, what is going on here? What should I do to get Hex elements on the Magenta colored region too? The new cae file is attached here - https://www.dropbox.com/s/452tdytz78lil3p/Mesh_pro...

Thanks in advance!

RE: Help meshing a complex part

Your single beam likely doesn't have exactly the same mesh on the different sides. Try cutting the beam with more of the symmetry planes available. The length can be cut in half. I think you can also cut it along the length once or twice. I hope this helps.

Thank you.

Rob Stupplebeen
OptimalDevice.com
My Personal WP

RE: Help meshing a complex part

You have a single part which presumably can be instanced several times and translated and rotated to make up the full assembly. If this part is a dependent part then you can mesh the individual part and hence make up the fully meshed assembly. On those faces in contact just tie the surfaces together. I'm not sure what you've done other than to possibly merge the parts together and so losing the structured region. I notice that with the hex mesh of the single part has elements that are badly distorted which will give warning messages.

RE: Help meshing a complex part

(OP)
Hi corus, Can you suggest any other option to have un-distorted elements at those regions?

RE: Help meshing a complex part

There's not a lot you can do given the angles in the part. Refining the mesh doesn't help either though for an arc you should be looking at an element size that subtends at least 15 degrees. Your mesh looks too coarse for that criteria. Warning messages on element shape aren't necessarily a bad thing but if you want to avoid them altogether then use tet elements and pay the price for a more expensive model to run.

RE: Help meshing a complex part

(OP)
Hi corus, Its impossible to get Hexa mesh without at least 5% elements showing warning. So I used all Tets, but the Force-Displacement gives higher resisting force than it should be. I have read on Abaqus manual that C3D4 Tets are stiffer than C3D8 Hex elements. So should I use the Hex elements despite the warning messages?

RE: Help meshing a complex part

(OP)


This way? But it still shows the Tet element as C3D4.

RE: Help meshing a complex part

Click on the Quadratic option.

RE: Help meshing a complex part

(OP)
Quadratic means C3D10M, which gives 70% elements warning!

RE: Help meshing a complex part

I meshed the original assembly of a single part using a mesh size of 1e-4 and the mesh verification said there were no elements to produce errors or warnings. It did give 37000 elements though.
I'd try the hex elements and put up with the warning messages and check to see if your results look reasonable. You could also use a simple static test case to compare the results with a tet mesh before moving on to do the explicit analysis.

RE: Help meshing a complex part

An alternative would be to use a mix of tet elements and brick elements. The regions that produce poor hex element shapes (mostly at the tips of the parts) could be meshed using tet elements, and the other regular regions meshed using hex elements. The connecting surfaces between tet and hex elements are automatically tied together. This gets rid of any warning messages and reduces the number of elements and nodes. The problem with this approach is you get a discontinuity in your results at the connecting surface which is ok-ish if the connecting surface is away from regions of interest.

RE: Help meshing a complex part

I tried downloading the file(s) but it seems to have disappeared. Anyway, why can't one-sixth of the geometry of one of these bars be meshed with linear bricks first? At least a few partitions in the bars seem unnecessary, by the way. Once one bar is meshed, it is a matter of playing with mirroring, merging nodes, etc. to get the final mesh of one bar. And then you repeat essentially the same procedure to get your final desired mesh.

Are you new to this forum? If so, please read these FAQ:

http://www.eng-tips.com/faqs.cfm?fid=376
http://www.eng-tips.com/faqs.cfm?fid=1083

RE: Help meshing a complex part

(OP)
Hi corus,

I guess it would be better to use both Tet and Hex elements and see which one performs better. I am mirroring the single part to get a new part with 3 single parts, but unable to delete the top one (Double mirroring gives 4 parts). I have tried partitioning the top part and delete it but it does not work, it just deletes the mirrored region (top 2 parts in this case).



Could you please look into it?

RE: Help meshing a complex part

Export the geometry to SolidWorks or CATIA or something, edit the geometry there and then import the edited geometry back in to CAE. In a recently faced situation, I realized that partition deletion in CAE isn't as intuitively simple as I was hoping it should be.

Are you new to this forum? If so, please read these FAQ:

http://www.eng-tips.com/faqs.cfm?fid=376
http://www.eng-tips.com/faqs.cfm?fid=1083

RE: Help meshing a complex part

(OP)
I tried SpaceClaim (my default CAD software), but meshing fails upon importing to ABAQUS.

RE: Help meshing a complex part

Instance the single part a few times and then translate the copied parts and constrain them to match faces until you've built the full assembly.

RE: Help meshing a complex part

I feel like this is a doable task for Abaqus/CAE. As I mentioned above, unless I am missing something, you could even instance 1/6th of the geometry of just ONE bar and then use the operations a bunch of us have been suggesting.

Could you please upload the geometry file (in one of the Abaqus/CAE-friendly formats)? I tried the link provided above but the file seems to have disappeared.

Are you new to this forum? If so, please read these FAQ:

http://www.eng-tips.com/faqs.cfm?fid=376
http://www.eng-tips.com/faqs.cfm?fid=1083

RE: Help meshing a complex part

(OP)
Hi IceBreakerSours, The file has moved here - https://www.dropbox.com/s/40zjjq8dikyxhoh/Mesh_pro...

Is there anyway I can do this (Mirroring and deleting partition) in Part module only? Actually I don't want to achieve this through Assembly module.

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