CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > ANSYS

Combining Hex and Tetra Mesh

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   October 13, 2011, 07:38
Default Combining Hex and Tetra Mesh
  #1
New Member
 
ZenCef
Join Date: Feb 2010
Posts: 22
Rep Power: 7
ZenCef is on a distinguished road
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.
Attached Images
File Type: jpg 1.jpg (95.5 KB, 52 views)
File Type: jpg 2.jpg (58.5 KB, 36 views)
File Type: jpg 3.jpg (94.4 KB, 38 views)
File Type: jpg 4.jpg (100.2 KB, 44 views)
File Type: jpg 5.jpg (59.6 KB, 35 views)
ZenCef is offline   Reply With Quote

Old   October 19, 2011, 10:02
Default
  #2
New Member
 
ZenCef
Join Date: Feb 2010
Posts: 22
Rep Power: 7
ZenCef is on a distinguished road
Any ideas ?
ZenCef is offline   Reply With Quote

Old   November 2, 2011, 15:29
Default
  #3
Member
 
jonathan
Join Date: Jun 2009
Posts: 47
Rep Power: 9
jonny_b is on a distinguished road
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 is offline   Reply With Quote

Old   November 2, 2011, 15:29
Default
  #4
Member
 
jonathan
Join Date: Jun 2009
Posts: 47
Rep Power: 9
jonny_b is on a distinguished road
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...."
jonny_b is offline   Reply With Quote

Old   November 3, 2011, 02:25
Default
  #5
New Member
 
ZenCef
Join Date: Feb 2010
Posts: 22
Rep Power: 7
ZenCef is on a distinguished road
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 ?
ZenCef is offline   Reply With Quote

Old   November 4, 2011, 16:15
Default
  #6
Member
 
jonathan
Join Date: Jun 2009
Posts: 47
Rep Power: 9
jonny_b is on a distinguished road
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 is offline   Reply With Quote

Old   November 4, 2011, 16:21
Default
  #7
Member
 
jonathan
Join Date: Jun 2009
Posts: 47
Rep Power: 9
jonny_b is on a distinguished road
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?
jonny_b is offline   Reply With Quote

Old   November 10, 2011, 06:04
Default
  #8
New Member
 
ZenCef
Join Date: Feb 2010
Posts: 22
Rep Power: 7
ZenCef is on a distinguished road
Quote:
Originally Posted by jonny_b View Post
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 View Post
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.
ZenCef is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
[ICEM] how to mesh a sail (and the rest of the boat) matteoL ANSYS Meshing & Geometry 4 May 7, 2012 10:23
[ICEM] A question about model an architechture about vetilation sunnyonly ANSYS Meshing & Geometry 4 September 23, 2010 11:33
Change parameters for Hybrid mesh karananand ANSYS Meshing & Geometry 3 July 18, 2010 16:37
Urban scenario - tetra vs hex problem pablocg OpenFOAM Running, Solving & CFD 6 April 9, 2009 03:14
Difference between Hex and Tetra in CFX massimo CFX 21 October 24, 2006 08:06


All times are GMT -4. The time now is 08:08.