×
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

How to refine an axisymmetric mesh in the contact region ?

How to refine an axisymmetric mesh in the contact region ?

How to refine an axisymmetric mesh in the contact region ?

(OP)

Hello,

I am studying sharp indentation on a quarter cylinder corner in Abaqus and I am not satisfied with my mesh, which is currently using Tet elements (with edge seeding in the corner). I would like to use bricks (Hex element) and refine the mesh in the contact region. I already tried several solutions with the Bottom-up and "classic" mesh tools. But I don't know how to create fine transitions between each region.

I attached a picture of the partitioned mesh (with zooms on transitions) I would like to obtain.

Does anybody know how to do that ?

Thank you very much

Best,

--
McFly M.
 

RE: How to refine an axisymmetric mesh in the contact region ?

You could model seperate parts and tie them together, then you can mesh each part with a different mesh density.

Or, you could use bias meshing, where you define a high number of elements in the contact zone and less in the areas you are not so concerned about.

Hope that helps.

RE: How to refine an axisymmetric mesh in the contact region ?

hello,

My suggestion is also in line with fruton.

I model seperate parts and tie them together and use bias mesh.(mapped mesh)

thanks,

RE: How to refine an axisymmetric mesh in the contact region ?

A smooth transition between mesh densities is the best option rather than a sudden jump in mesh as this will cause irregularities in the solution at the transition. Use biasing and play around with the various options in CAE for 2D Quad meshing rather than using the structured meshing you have.  

Tara

http://tinyurl.com/4ydjg7m

RE: How to refine an axisymmetric mesh in the contact region ?

(OP)

Thank you very much for your answers, I'd better not use different parts to avoid discontinuities but I have really been trying a lot of different options of meshing. But nothing really satisfying.

There must be a way to create the smooth transitions as seen in the attached picture in my first message. Besides, this time I attached a file where we can see the same type of (trapezoidal) elements at the transition between both regions. This figure comes from "Getting Started with ABAQUS/Standard", fig.4-43, "Mesh refined around the hole". I would like to get a similar mesh (with inverted convexity of course).

Any suggestion ?

--
McFly

RE: How to refine an axisymmetric mesh in the contact region ?

Have you tried partitioning the model to achieve what you want?

RE: How to refine an axisymmetric mesh in the contact region ?

(OP)
yes, but CAE refuse to mesh my partition with Hex-elements using the classic mesh tool. I also tried Bottom-up mesh (Revolve) but it won't mesh probably because he can't tie each region's mesh due to the gap of density.

RE: How to refine an axisymmetric mesh in the contact region ?

Here is a running list of questions and comments:
1. Why not axisymmetric?  I was under the impression that the loading was non-axisymmetric otherwise I would have suggested it earlier.
2. The part name is cheese are you really modeling the indention of cheese?!?
3. Since you have switched to tets you can use adaptive remeshing to refine the mesh locally based on the loading.
4. Use quadratic Tets or Hex
5. A biased edge seed appears to work well.  I tried 20 global and for the 3 edges near indention bias 20 on the peripheral side and 0.5 near contact. (See image)
6. Nonlinear geometry should be used when contact or plasticity are used.  It is not turned on in the preload step.
7. What does the preload step do?  Is this legacy?

If I get the time I will try running this model.  I hope this helps.

Rob Stupplebeen
https://sites.google.com/site/robertkstupplebeen/

RE: How to refine an axisymmetric mesh in the contact region ?

(OP)
Hi,

Thank you for your help. I already tried a similar mesh but I would really like to mesh with Hex.

To answer your questions
1. Indeed the load could be non-axisymmetric, that is the point of my work.
2. Cheese is just a funny name I gave to my part. (I'm french...)
3. We are not very into adaptative meshing (yet).
4. Yes, I will once I have made the initial verification of my model.
5. Well, thanks, it is good to know.
6. Ok, I will fix this. I am sorry but I don't get what the non linear geometry option does exactly. Has it something to do with large deformation?
7. I study the influence of residual stresses on indentation testing, the point of the preload step is to impose a non-axisymmetric displacement (for the moment it's just a pressure but I will fix this too).

The model is 200 times bigger than the contact region, the purpose was to avoid the boundary effects on the elastic calculations. It could be smaller using plastic.
 

RE: How to refine an axisymmetric mesh in the contact region ?

(OP)
Sorry, I actually didn't try the Bias tool. I will play around this feature and see if I get something satisfying.

Best

RE: How to refine an axisymmetric mesh in the contact region ?

(OP)
I finally found a pretty satisfying mesh and managed to achieve very good results with it.

I am now confronted with another problem. I would like to take non-equi biaxial residual stresses into account and study their influence. Therefore I would like to subject the lateral surface of the cylinder to a displacement. I tried 2 solutions :

1) I defined 1 BC (displacement) on the lateral surface (Ux=1/Uz=1)

This is obviously incompatible with the other BCs (symmetry->no normal displacement on faces Z0Y & X0Y). So when I try to run the job I get this kind of message :

"31 nodes have dof on which velocity/displacement/acceleration/base motion etc. constraints are specified simultaneously. The nodes have been identified in node set ErrNodeBCRedundantDof." So I tried another solution :

2) I defined 2 BCs (displacements): one for Ux and the other one for Uz, I also defined 2 analytical fields so that Ux is proportional to X (and Uz to Z). This way there are no conflict between symmetry BCs and "load" BCs.

But still I get the same message. It seems that there is still a conflict in the fact that I impose the same the constraint twice at the same place.

Is there a way to avoid this ?

(I already tried to impose a pressure on the lateral surface and it worked but that is not the point of my study, unfortunately...)

--
MF       

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