CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Mesh Generation & Pre-Processing Software > ANSA

Hybrid Hexa-Tetra Mesh in ANSA

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

Like Tree1Likes
  • 1 Post By tomf

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   May 27, 2016, 06:40
Default Hybrid Hexa-Tetra Mesh in ANSA
  #1
New Member
 
Join Date: May 2016
Posts: 3
Rep Power: 8
SebastianK589 is on a distinguished road
Hi everyone,

I have to establish a Hybrid Mesh with a structured Zone with Hexa elements and an unstructured Zone with Tetra Elements.

I`m used to ICEM and now have to use ANSA. I want a conformal interface between those two zones.

Can anyone help me here ?

Kind regrads,

Sebastian
SebastianK589 is offline   Reply With Quote

Old   May 30, 2016, 04:41
Default
  #2
Senior Member
 
Tom Fahner
Join Date: Mar 2009
Location: Breda, Netherlands
Posts: 606
Rep Power: 30
tomf will become famous soon enoughtomf will become famous soon enough
Send a message via MSN to tomf Send a message via Skype™ to tomf
HI,

In that case I would create the structured zone first. It depends on your geometry what would be the best way to do this (Hexablock, layer extrusion, revolve). Make sure you have a surface with quads (geometry or FEM) on the interface between both zones. Then automatically detect the remainder of the domain and mesh it with tetra rapid. You will get pyramids right next to the interface, due to fact that it needs to be conformal.

Regards,
Tom
vangelis likes this.
tomf is offline   Reply With Quote

Old   March 6, 2017, 08:51
Default
  #3
New Member
 
Join Date: Mar 2016
Posts: 29
Rep Power: 8
The_Kaiser is on a distinguished road
I had a similar thing to do. The problem is now, betwenn the structured and unstructured part I have a layer of 2D-elements, which are exporting into OpenFOAM, even if I don't define them into PID's. Can I make them disappear somehow?
The_Kaiser is offline   Reply With Quote

Old   March 7, 2017, 05:13
Default
  #4
Senior Member
 
Vangelis Skaperdas
Join Date: Mar 2009
Location: Thessaloniki, Greece
Posts: 286
Rep Power: 19
vangelis is on a distinguished road
Hi Kaiser,

If you start ANSA in CFD layout you will see that in the Property List there is a column "Use In Model". By default for the Property "Top_Cap_Layers" the surface mesh between the layers and the unstructured mesh, this setting is OFF, which means that in output it will not be written.
Make sure also that you have the same Property for the layers and the unstructured volume before output. Use Volumes>SET PID select the two volumes and place them in a Property called "Fluid" for example.

Hope this helps
Vangelis
vangelis is offline   Reply With Quote

Old   March 9, 2017, 05:03
Default
  #5
New Member
 
Join Date: Mar 2016
Posts: 29
Rep Power: 8
The_Kaiser is on a distinguished road
Ok, that's done. But right now a new problem problem appeared, that wasn't a problem earlier

I first created my structured mesh, then my unstructured. First time, I used Shell Mesh -> Intersect -> Solid Description and the volume meshes merged fine together. Now they don't want to. If I generate Shell Meshes on the Volumesn, the Intersect option don't merge the voumes. How can I merge the 2 volume meshes in an easy way?
The_Kaiser is offline   Reply With Quote

Old   March 9, 2017, 05:11
Default
  #6
Senior Member
 
Vangelis Skaperdas
Join Date: Mar 2009
Location: Thessaloniki, Greece
Posts: 286
Rep Power: 19
vangelis is on a distinguished road
Hi Kaiser
When you generate the layers, ANSA generates the top cap shell mesh by default. Then you press Define Auto Detect and ANSA detects the rest of the volume to be meshed with unstructured mesh. You then MeshVolume TetraRapid for example and ANSA creates the unstructured mesh.

You do not have to do anything to connect these two volumes together. They are already connected as they share the same surface mesh of the top cap.

You only need to use Volumes>SET PID select them both and put them in 1 Property.

Then output, ANSA will output the surface and volume mesh, but NOT the topcap shell mesh as this is by default Use in Model NO.

The function Intersect>Solid description has nothing to do with volume mesh.

Hope this helps
Vangelis
vangelis is offline   Reply With Quote

Old   March 9, 2017, 05:42
Default
  #7
New Member
 
Join Date: Mar 2016
Posts: 29
Rep Power: 8
The_Kaiser is on a distinguished road
Thanks for the fast answer.

The problem is, I want to generate a mesh for a tire in a box. I generate the tire 2D-structured mesh in the XY-plane and extrude in Z direction. But when I do what you say, ANSA says that I need a surface mesh on the tire surface (the surface that would be in contact with ground-but here it's just in the air). When I now generate a 2D-Mesh on the tire surface with Map, how can I be sure, that it's connected with the 3D-extrusion? ANSA checks Manager says, that I have intersections.

Thanks in advance for your help
The_Kaiser is offline   Reply With Quote

Old   March 9, 2017, 07:22
Default
  #8
Senior Member
 
Vangelis Skaperdas
Join Date: Mar 2009
Location: Thessaloniki, Greece
Posts: 286
Rep Power: 19
vangelis is on a distinguished road
Could you please send an image of the problem so that I better understand the case?
vangelis is offline   Reply With Quote

Old   March 12, 2017, 11:30
Default
  #9
New Member
 
Join Date: Mar 2016
Posts: 29
Rep Power: 8
The_Kaiser is on a distinguished road
[img] https://www.dropbox.com/s/gqv8l2qm5o...2046.jpeg?dl=0 [/img]

Inside of the blue circle I want to have a structured mesh. I make an O-Grid in XY-plane and extract it in Z-direction. But now I don't have a surface mesh on my blue surface (right pic). It's just a volume mesh. And I'm not sure how to make the surface mesh so that everything will fit fine.

Thanks in advance, sorry for the late answer, exam time

Last edited by The_Kaiser; March 12, 2017 at 11:41. Reason: pic ^^'
The_Kaiser is offline   Reply With Quote

Old   March 13, 2017, 04:27
Default
  #10
Senior Member
 
Vangelis Skaperdas
Join Date: Mar 2009
Location: Thessaloniki, Greece
Posts: 286
Rep Power: 19
vangelis is on a distinguished road
I am not sure i understand what you try to do, but to answer your simple question, how to create shell mesh on top of free volume mesh,
use Mesh>Elements>Vol-Shell [Skin]
Activate the feature angle selection tool, pick one free volume facet and ANSA will pick all neighboring facets within the specified feature angle.
vangelis is offline   Reply With Quote

Old   March 13, 2017, 16:26
Default
  #11
New Member
 
Join Date: Mar 2016
Posts: 29
Rep Power: 8
The_Kaiser is on a distinguished road
It worked somehow with your previous advices. I'm not sure how and why, but with my slow pc I didn't want to screw it up, while figuring it out. Thanks a lot for your help!
The_Kaiser is offline   Reply With Quote

Old   March 14, 2017, 02:47
Default
  #12
Senior Member
 
Vangelis Skaperdas
Join Date: Mar 2009
Location: Thessaloniki, Greece
Posts: 286
Rep Power: 19
vangelis is on a distinguished road
You are welcome
vangelis is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
DES case - instability with Hexa Mesh greg.cfd OpenFOAM Running, Solving & CFD 3 May 9, 2018 11:18
[ICEM] Hexa mesh, curve mesh setup, bunching law Anorky ANSYS Meshing & Geometry 4 November 12, 2014 01:27
[ANSYS Meshing] Are there any drawbacks to a hybrid mesh? JuPa ANSYS Meshing & Geometry 4 April 22, 2014 11:33
[Other] hexa vs hybrid mesh convergence Viais OpenFOAM Meshing & Mesh Conversion 0 April 23, 2010 11:39
fluent add additional zones for the mesh file SSL FLUENT 2 January 26, 2008 12:55


All times are GMT -4. The time now is 21:26.