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] Prism (http://www.cfd-online.com/Forums/ansys-meshing/113787-prism.html)

potiolot February 26, 2013 13:39

Prism
 
1 Attachment(s)
Dear all,

I'm have a new user of the prism mesh generator in ICEM (some experience with tetra).

My geometry is very simple (a 3D cube of size 3000x400x50) in which a very small source of height 0.1 is enclosed and must be precisely meshed.

I never succeed in generating a correct prism mesh (see the enclosed caption). The prisms layers are disappearing exactly where the small body is defined...

I first generated a 2D triangle mesh and then tried to apply the prism mesh generator on the 2D mesh (with top faces selected for prism layers).
No properties were defined on curves.

Any help would be more than welcomed.

Thanks for your attention,

Fabien

PS : Is there any very simple tutorial with prism mesh?

Far February 26, 2013 23:47

Why not to try ICEM HEXA for precise control?

potiolot February 27, 2013 02:48

Hello,

Thanks for your reply.
However, our CFD code only handles tetras or prisms.

Any idea?

Best regards,

Fabien

potiolot February 27, 2013 02:50

And by the way, we don't have any license for hexa...
Fabien

BrolY February 27, 2013 03:08

To which part does the curve of the green surface belong ?

Maybe you should add this curve to the blue part, so the prism should know they can propagate on this curve too.

diamondx February 27, 2013 10:53

you forgot to check prism for that part too...

kad February 27, 2013 11:49

5 Attachment(s)
I think the problem is that prism canīt handle the small height of the source. So here is a approach by using the extrude mesh function. With this method you can generate an all prism mesh and have very good control of your mesh sizes. It works as follows:

- set up your geometry
- generate (patch dependent) surface mesh for the bottom of your domain
- extrude surface mesh to the top of the source
- extrude from top of source to top of domain

To explain the method I have made a little box in a box geometry which you can see in attachment 1.

1) We want to extrude the surface along curves so these curves have to be defined. For the first extrusion a curve of the inner box can be used. For the second extrusion we need an curve from top of the inner box to the top of the domain. The easiest way is just to use the project point to curve with the trim option enabled. Also be sure to have a material point in each closed volume, in this case two.

Then the node distributions for the two curves are defined under "curve mesh setup" which will give you the number of extruded layers. See attachment 2.

2) Generate a surface mesh for the bottom of the domain. Here make sure that you capture all of the bottom, also the inner of the small box (attachment 3). For best result and control use patch dependent meshing.

3) In the next step the surface mesh is extruded to the top of the small box. We want to use the method "Extrude along curve" and as spacing type "curve bunching". Check the curve directions and reverse them if necessary. Pick the first extrusion curve and select all visible elements. As "new top part name" choose a default name like "tmp" and keep the rest on "inherited". Then extrude the mesh (attachment 4).

4) Same as above. Choose the new extrusion curve and as elements select all elements in the just created part "tmp". Extrude the mesh to the top of the domain (att5). No need to change any of the names for top or side.

Now the extrusion itself is done. Now, the mesh has to be edited to get rid of some unwanted faces and for correct associations.

I will continue in the following post due to limitation of the number of attached files.

kad February 27, 2013 12:05

5 Attachment(s)
5) In the next step the volume elements are assigned to their correct material points. For this use "mark enclosed elements" under edit mesh. Select for both inputs "all appropriate visible objects" from the selection menu (att6).

6) Delete the inner volume of the small box. Therefore enable volumes in the display tree with ONLY the part that contains the material point of the small inner volume. Then delete these volumes (att7). If you want to keep the inner volume skip this step.

7) For correct association of the shell elements we first want delete them all (att8).

8) The run the check mesh function. Of course, it will show you uncovered faces (att9). So you want to fix these. Assign them a new part like "uncovered". If you have not deleted the inner volume in 6) there will be additional "missing internal edges". Assign them a new part like missing, too.

9) Associate the just created shell elements to the geometry. Use the "Associate mesh with geometry" under edit mesh ->repair (same as mark elements). Pick only shell elements from the selection menu (att10).

kad February 27, 2013 12:10

1 Attachment(s)
10) Run checks and visually scan the mesh for right associations. If necessary correct them manually.

11) You have a nice mesh for simple geometry that is not hexa (att11).

Also with the patch dependent method you have almost full control of the mesh around your source or "inner box". A little disadvantage is, that the generated mesh is not one hundred percent body fitted.

Of course it works for hexa, too. Then you want to start with a allquad surface mesh.

potiolot March 1, 2013 08:54

Dear all,

Thanks for your answers, I will follow the methodology kindly given by Kad.

Best regards,

Fabien


All times are GMT -4. The time now is 01:15.