CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   ANSYS Meshing & Geometry (http://www.cfd-online.com/Forums/ansys-meshing/)
-   -   [ICEM] Uniform mesh in ICEM (http://www.cfd-online.com/Forums/ansys-meshing/84645-uniform-mesh-icem.html)

harerton February 4, 2011 10:39

Uniform mesh in ICEM
 
Hi everybody,

How do I get a uniform mesh with hexa elements of the same size in ICEM?

My domain has rectangular faces and all the elements are organized so that hexa elements with 2cm side would fit properly.

What are the correct parameters to be used?

Thanks!

BrolY February 4, 2011 11:55

Play with the "Edge Params" option (blocking -> Pre Mesh Params -> Edge Params).

PSYMN February 5, 2011 15:18

Automatic option...
 
Or you could try an automatic Cartesian method such as BFCart...

Can you post an image or maybe even your model and I could illustrate...

harerton February 6, 2011 00:21

1 Attachment(s)
I have attached the model.

The flow enters the domain through an inlet at one extremity, near some obstacles and exit through the other extremity.There's a cubic obstacle downwind the domain. The geometry parts are: INLET, OUTLET, RIGHT, LEFT, TOP and WALLS (which includes the floor and the obstacles surfaces).

What I do in ICEM:

1 - Import the geometry
2 - Create the parts
3 - In Mesh - Global Mesh setup:

a) Global Mesh Parameters: Global element seed size = 0.02m;
b) Shell meshing parameters: Mesh type = All Quad; mesh method = autoblock;
c) Volume mesh parameters: Mesh type = cartesian; mesh method =body-fitted; Aspect ratio 1 1 1;

4 - Compute volume mesh.

The generated mesh is all hexa, but the elements don't have all the same size on each face, while some of them aren't even cubes. Their faces are less than 0.02m.

I would like to get a mesh where every element is a cube with a 0.02m side!

Thanks for any help!

PSYMN February 19, 2011 21:14

BFCart.
 
2 Attachment(s)
You mixed two methods that don't mix. The Cartesian method is a top down method, which means you don't need to start from a surface mesh.

I will attach my tetin file of your model.

Like you, I setup parts and set all the sizes (including the global max size) to 0.02.

Then I made sure the Cartesian meshing parameters were setup and meshed with BFCart...

I got this. (Cutplane shown)

Attachment 6558

I have to say that I think this is not very efficient. Most users prefer to have more elements in the important areas and fewer elements in the less important areas. Uniform density is not what most people are looking for.

This could be very much improved by creating your own cartesian back ground grid with hexa (like is done in the femur tutorial).

If you want, you could also try Octree Tetra followed by a tet to hex conversion (very easy and popular way of getting hexa dominant mesh that transisitions well, converges well, etc.), or perhaps go for full blown hexa blocking (by far the best solution if your real model is this simple).

harerton February 20, 2011 09:25

Quote:

Originally Posted by PSYMN (Post 296089)
If you want, you could also try Octree Tetra followed by a tet to hex conversion (very easy and popular way of getting hexa dominant mesh that transisitions well, converges well, etc.), or perhaps go for full blown hexa blocking (by far the best solution if your real model is this simple).

Thank very much for your answer. I know uniform is not the best alternative. But I was trying to find a way to generating it.

Anyway, where do I find this femur tutorial? And are there tutorials for these two alternatives you suggested above (see quote)?

Thanks again!

PSYMN February 21, 2011 01:08

Tutorial.
 
This is a pretty old tutorial (2008 I think)... It was one I quickly put together for a hands on session at a conference... I got some complaints that i didn't include enough detail, such as how to use subsets to get the cutaway mesh views...

But hopefully you still get something out of it.

I think later the doc people turned it into a real tutorial and put it into the customer portal... You can look for that if you want, but here is my original.

ftp://ftp.ansys.com/outgoing/simon/ICEMCFD_Femur.zip

In this tutorial, instead of letting the software create its own cartesian background mesh, you can create it... This means you can align it perfectly with your far field (and not have it distort as it projects to surface). You can also used edge parameters to bias along the duct and reduce your mesh count in one direction...

Have fun.

harerton February 21, 2011 06:16

Thanks! Will take a look!

harerton February 22, 2011 07:32

Simon,

Thank you very much for all your help. With the aid of your tutorial I was able to understand more of how ICEM works and I was able to produce a much more improved mesh.

Thanks again and keep up the good work!

Harerton


All times are GMT -4. The time now is 11:17.