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/)
-   -   [GAMBIT] Issues with Cooper Volume Meshing (http://www.cfd-online.com/Forums/ansys-meshing/63235-issues-cooper-volume-meshing.html)

Forrest April 1, 2009 12:29

Issues with Cooper Volume Meshing
 
Hi all, I'm trying mesh the volume shown in the first picture using the Cooper Method. My source mesh is shown in the second picture. When I implement the Cooper scheme, Gambit generates negative volume cells (which can be seen in the mesh slices in Images 3 & 4). I really don't understand how gambit can mess the mesh up before it gets to the portion of the volume where the expansion starts since it is a straight pipe up till that point. I want the boundary layer mesh to maintain its dimensions the entire length of the volume.

I've tried to split this volume into two portions so that I would have one volume with the red face in Image 1 and one with the yellow faces. When I tried this I get the following message:

Quote:

ERROR: Attempted to split volume volume.2 using face v_face.23 that doesn't divide it into two parts (has edges not common with the volume).
I don't know how this could be since all I did was connect the two verticies of the semi-circle edge at the red/yellow junction with a real edge and make a virtual face using the new edge and the semi-circle edge.

Does anyone know what is going on with the Cooper scheme and/or know how to fix it? I am also open to alternative ideas on how to mesh this volume. Thanks in advance

http://lh6.ggpht.com/_-cnbldNBBl4/Sd...icture%204.png

http://lh4.ggpht.com/_-cnbldNBBl4/Sd...icture%201.png

http://lh5.ggpht.com/_-cnbldNBBl4/Sd...icture%202.png

http://lh3.ggpht.com/_-cnbldNBBl4/Sd...icture%203.png

-mAx- April 1, 2009 12:57

Hi Forrest,
The best way is to plit your volume in several volumes.
The first volume should be a pipe till the expansion.
Then you may mesh the other volume (not the pipe).
Don't try to mesh too fast (direct with BL), because when you split your domain you lost the BL.
So try to mesh with cooper the volumes, and then if all is ok, you can apply the BL.
For meshing the volume, mesh with quad-pave the smallest cap.
Then enforce the cooper scheme, with the right sources (small and big cap).
if it's not ok, try to resplit this volume, but it should be ok, it's like a conus.
Once this volume is meshed, propagate this mesh along the pipes.
But your problem is that your work with virtual volumes, so the splits aren't so simple.
Try this way: split edge --> split faces with the vertices produces from the edge splitting --> create the face with the generated edges and split the volume with the face.
In real volume, you would have to expand the face to be sure that the face split all the volume (I assume this is a tolerance issue).
I was face dto this problem today, and I solved it with this way
;)

Forrest April 1, 2009 16:13

Ok, I was able to split my "pipe" volume into two pieces (the blue and red one in the image). I was able to mesh the straight pipe volume succesfully with the cooper scheme without generating any highly skewed cells or inverted cells. (I meshed each volume separately)

Unfortunately I was so lucky with the expansion part. I think this is because I have a lot of points clustered near one end of the semi-circle so that I can better capture an exit jet in the straight pipe portion. I am correct in assuming that I will have to split this volume up into smaller volumes to mesh it properly?

I had a question regarding your suggestion about the BL meshes. You said:
Quote:

So try to mesh with cooper the volumes, and then if all is ok, you can apply the BL.
How do I apply the BL mesh to something I already have meshed? Should remove the volume mesh and redo my source face mesh to include a BL mesh and then remesh the volume? Thanks

http://lh3.ggpht.com/_-cnbldNBBl4/Sd...icture%206.png

http://lh3.ggpht.com/_-cnbldNBBl4/Sd...cture%2014.png

-mAx- April 1, 2009 17:13

yes you can mesh your volume, then apply the BL and remesh the volume.
Regarding the expansion, I saw on the 2nd picture that you have a small edge on the front surface (which generates a poor surface mesh quality).
Try following steps:
split the opposite edge, and reproduce the same small edge (but at the opposite)
split the face with those 2 vertices.
Your surface is now splitted into 2 surfaces (one is a rectangle)
Extrude this edge along the y-axis, and split the volume.
In other words do the same procedure as here:
http://www.cfd-online.com/Forums/ans...on-w-pics.html

Forrest April 3, 2009 17:46

Ok, I split the volume of my entire pipe volume (including the expansion) like you suggested by make a small rectangular volume to deal with the clustering (I also split the expansion volume in half). I am able to generate a mesh with no skewed cells (>0.97) and and no inverted elements with just a paved triangular source face. However everything goes down the drain when I try use a source face with a boundary layer mesh (on the small semi-circle face). Everything works great as it goes through the straight portion of the pipe, but gambit has some real problems when it tries to mesh the region where it goes from a circular pipe to the expansion (highly skewed elements and inverted elements are formed). Is applying the BL mesh to the source face the best way to go about applying the BL mesh, or should I try to attach a BL mesh to the face?

-mAx- April 4, 2009 03:11

If you want to have an cooper mesh on the expansion, Gambit will take the small cap as source and will patch it on the expanded cap.
So I think you will have degenerated cells because of the brutal expansion.
If you absoloutely want to deal with hexa you will have to split the volume in small ones along the axis (for a better control of the expansion).
Or you can mesh it with tetra-hexcore (tetra outer layer with hexa core) and you may apply a size function on the small cap.
As I said you may deal with the BL once all the splits etc are done... (but maybe I'm wrong)


All times are GMT -4. The time now is 21:09.