CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   ANSYS (http://www.cfd-online.com/Forums/ansys/)
-   -   Combining Hex and Tetra Mesh (http://www.cfd-online.com/Forums/ansys/93377-combining-hex-tetra-mesh.html)

ZenCef October 13, 2011 07:38

Combining Hex and Tetra Mesh
 
5 Attachment(s)
Hi Guys,

I need to combine hex and tetrahedral mesh. I have two volumes and they formed in same part. In figure 1 and 2 volumes are shown. As you can see in figures a pipe is connecting with a annular volume. I want to add infilation to pipe. Becouse of hexahedral infilation, highly skewed cells are formed in connection area. You can see the meshes and skewed cells in figure 3,4 and 5. Could you give me an advice about meshing the connection area. By the way i tried the body sizing with sphere of influence to the connection area but it doesnt decrease the skewness.

Best regards.

ZenCef October 19, 2011 10:02

Any ideas ?

jonny_b November 2, 2011 15:29

If you are using ANSYS Meshing to mesh this geometry. Is so are you trying to mesh each body simultaneously? What you could do is use direct meshing (avail. in v13 and above) and mesh the pipe with inflation first. Then mesh the annulus second. By doing this the surface topology at the interface is unchanged and the tetra mesher will be forced to mesh around this interface. If you have highly skewed cells you can try reducing the size of your elements at the interface between the pipe and annulus. Also try adding a body sizing control with a smaller value for the growth rate of the body.

jonny_b November 2, 2011 15:29

Sorry I noticed my typos in my first two sentences. They should read: "Are you using ANSYS Meshing to mesh this geometry? If so are you...."

ZenCef November 3, 2011 02:25

Thanks for your reply jonny_b... I meshed both simultaneously and part by part for using direct meshing. As you say, i meshed the pipe with inflation first then mesh the annulus second. After that i use body sizing for both part with sphere of influence but pipe side with inflation doesnt change. Anyway i'll try again... Is there any tutorial or something like that about meshin like this parts ?

jonny_b November 4, 2011 16:15

Hmmm... this is strange indeed. I would think that this goemetry isn't that difficult to cause issues with meshing. I'm suprised that direct meshing with meshing the pipe first isn't working.

A few questions:
1) When you say you are using a HEX does that mean that you are using a swept mesh in the pipe with "all quads" selected? If so try changing to all tri or quad/tri and see what that does.

2) Also if you are using a swept mesh, are you defining your source and target faces manually. If not try manually defining these with the source being your interface between the domains and target being the other end of the pipe.

I do not know of any tutorials for this type of situation. My next suggestion would be to submit a service request through the ANSYS Customer Portal. You will have to create an account if you do not already have one. They application engineers who can be pretty good at diagnosing the issue.

jonny_b November 4, 2011 16:21

I just had a possible Ah ha moment. In the 4th figure you are showing a close up of the interface between the two domains. You're problem might be that your interface occurs right at the outlet of the pipe. I have had trouble in the past with an interface at the outlet of ducts. Try moving your interface upstream of the pipe such that part of the pipe is meshed with tetrahedrons and apply an inflation layer to this region of the pipe also. And second, when you say highly skewed is the maximum skewness value you are getting?

ZenCef November 10, 2011 06:04

Quote:

Originally Posted by jonny_b (Post 330773)
Hmmm... this is strange indeed. I would think that this goemetry isn't that difficult to cause issues with meshing. I'm suprised that direct meshing with meshing the pipe first isn't working.

A few questions:
1) When you say you are using a HEX does that mean that you are using a swept mesh in the pipe with "all quads" selected? If so try changing to all tri or quad/tri and see what that does.

2) Also if you are using a swept mesh, are you defining your source and target faces manually. If not try manually defining these with the source being your interface between the domains and target being the other end of the pipe.

I do not know of any tutorials for this type of situation. My next suggestion would be to submit a service request through the ANSYS Customer Portal. You will have to create an account if you do not already have one. They application engineers who can be pretty good at diagnosing the issue.

Hi Jonny_b, I couldn't deal with the matter for a while. For your questions,

1) I use sweep or patch conforming tetrahedrons method with "all tri" for the pipe. I wrote "hex" becouse after the inflation cells looks like hexahedral at inflated area as you can see at img 4.

2) When i use sweep mesh, i defined source & target manually becouse inflation problem. I couldn't get but when i define s&t automatically, inflation doesn't work. :)

Quote:

Originally Posted by jonny_b (Post 330775)
I just had a possible Ah ha moment. In the 4th figure you are showing a close up of the interface between the two domains. You're problem might be that your interface occurs right at the outlet of the pipe. I have had trouble in the past with an interface at the outlet of ducts. Try moving your interface upstream of the pipe such that part of the pipe is meshed with tetrahedrons and apply an inflation layer to this region of the pipe also. And second, when you say highly skewed is the maximum skewness value you are getting?

Thanks for your possible Ah ha moment :) I couldn't write for a while becouse i trying that. I was trying mesh with forming the bodies as new part. Now i united the pipe and annulus. Then i only generated mesh with priximity and curvature method, inflated by sellecting pipe surface. At the end of meshing max skewness is obtained as 0.855... I guess the value is ok for this geometry what do you think? And now i must obtain this skewness value for similliar 3 model for compare... Thanks for your help, i'll try and write the final situation.


All times are GMT -4. The time now is 16:03.