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

Developing Multi-Region Conformal Mesh

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

Reply
 
LinkBack Thread Tools Display Modes
Old   January 31, 2012, 22:13
Default Developing Multi-Region Conformal Mesh
  #1
New Member
 
Paul Kirchner
Join Date: Dec 2011
Posts: 11
Rep Power: 5
pkirchner is on a distinguished road
Hey there, I'm having trouble developing a conformal mesh on my multi-region interfaced boundaries. I've tried multiple meshing models, and combinations, but I get a (non-closed Volume) error when generating the volume mesh using all but the surface wrapper.
The only time I can get a mesh generated between the regions is when i use multi-region meshing within the surface wrapper....this however produces a non-conformal mesh.
Now I did find the (using the Use Conformal Face Match Only Option instruction in the help menu) -> surface repair tool-> merge/imprint, but the help menu doesn't really give good instructions on doing so.

I'm measuring flow rate on the porous baffle interface...when ran a previous simulation that had a conforming mesh via (polyhedral,surface remesher, extruder) I got .93 kg/s.
I then remeshed the part doing multi-region surface wrapping, which developed a non conformal mesh I got .82 kg/s. I cannot have this much error between iterations.
Does anyone have experience using the conformal match only option? or any experience conforming meshes by another means?
Attached Images
File Type: jpg NonConformalPolyMesh.jpg (91.6 KB, 111 views)
File Type: jpg NonConformalTrimmerMesh.jpg (104.1 KB, 81 views)
pkirchner is offline   Reply With Quote

Old   February 1, 2012, 13:20
Default
  #2
New Member
 
Paul Kirchner
Join Date: Dec 2011
Posts: 11
Rep Power: 5
pkirchner is on a distinguished road
PrintScreen of Conformal Face Window.... I'll run you all through what I'm attempting to do.

I have a over body flow simulation. I'm trying to simulate the flow through the sidepod modeling the radiator and fan.
What I've attempted:
Boolean subtract operation on all parts including the radiator, and fan...which have duplicates and are represented by generic solids. I send the Subtract (air) to it's own region. It has boundaries for both inlet and outlet of the radiator, and inlet and outlet of the fan. I then send the fan, and radiator to their regions. I do a Porous Baffle interface on the front side of the radiator, and a fully developed interface on the back side. I then interface the front and back side of the Fan in the same manner, but set it to a fan interface.
I've been using a Poly mesh with a 80mm base size, and volume refinement to 40mm on the air region.
I've attempted multiple meshes, and per region meshing to no avail.
I've also attempted to bring in only the sidepod/body part. I then created a new part from the curves where the fan would be located and where the radiator would be located. I then assign the sidepod/wind tunnel to it's own region, and the fan and radiator to their own. When I generate the surface mesh there are gaps between the edges...I tried to refine the fan/radiator mesh, but when I generate the volume mesh it has an open volume error, or non-manifold edges which would be expected.
I've also tried to do the same boolean process like the first attempt, but I combine the radiator, shroud and fan into one solid...set the front side as the porous baffle interface, and back side as the fan interface. I also get (open volume) error in this case. Anyone have any input? It would be greatly appreciated. Thanks!
Attached Images
File Type: jpg ConformalMeshingRepair.jpg (54.5 KB, 92 views)
pkirchner is offline   Reply With Quote

Old   February 1, 2012, 18:33
Default
  #3
Member
 
Join Date: Feb 2011
Location: DE-PB
Posts: 56
Rep Power: 6
willimanili is on a distinguished road
Try this one:

Create all your parts with boolean operations at the parts level. The resulting parts should not intersect each other. After this launch the surface repair tool for the parts you want to use for regions later on (load them all together to the surface repair). Then choose Merge/Imprint at the top of the surface repair tool window.
Select multi-region imprint. Click on Find pairs. Now all the part contacts should be found which will be your interfaces later on. You can now imprint each pair. Do it step by step and not by clicking on Imprint all. After each imprint you can go back to surface repair (at the top of the window) and start a diagnostic (non-manifold or free edges/vertices) to check if your imprint operation caused any problems. If it doesnt do the same for the next imprint pair. If it does you can try to fix these problems by changing the imprint tolerance value or sometimes it helps already to switch destination and source.
If all your parts are successfully imprinted you can assign them to regions. Interfaces will be build automatically if it isnt deselected. Apply your physics continua to your regions. You can now change the interface types if necessary. I think you use just one mesh continuum for all your regions?!
Create your surface mesh. Check your surface mesh for any nonmanifold or free edge issues and also if your interfaces are generated as you want it to. Usually all should be fine and you can go on with volumemeshing and setting up your simulation.
willimanili is offline   Reply With Quote

Old   February 1, 2012, 22:31
Default
  #4
New Member
 
Paul Kirchner
Join Date: Dec 2011
Posts: 11
Rep Power: 5
pkirchner is on a distinguished road
Thanks for the reply, still no luck however. I've successfully done this multiple times for the radiator, which is a 9"x13"x2" rectangle. When I locate the 4 pairs for the radiator it successfully pairs on each face. Now when I try it with the fan a 8"x 0.5" circle it finds a hundreds of pairs....not just the simple .5" edge around the circle..and the two 8" faces.

I have a feeling it's my geometry...and the original imported surface. Both the sidepod, and (fan) were created in Pro/E 5 using the same references, so the geometry should match..Any suggestions? different file type? I'll make the same drawing in the morning, but use a square with the same area as the circle for the output...and we'll see how it does. Any input is greatly appreciated. Thanks.

edit* the attachment are the imprint pairs found within the repair tool when I did it on the radiator.
Attached Images
File Type: jpg coincideimprint.jpg (85.6 KB, 42 views)
pkirchner is offline   Reply With Quote

Old   February 1, 2012, 23:04
Default
  #5
Senior Member
 
Join Date: Mar 2009
Location: Austin, TX
Posts: 134
Rep Power: 9
kyle is on a distinguished road
It could be some quirk of your input surface triangulation that is tripping up the remesher. Since it works if you use the wrapper, try doing just a wrap/remesh of each of your regions. Then, delete all representations other than the new remeshed surface. Repair the remesh representation and imprint the faces that you want to be conformal. Then set up the mesh continuum to do a conformal remesh and volume mesh. If that doesn't work, then you know it has to be something funky with your settings.
kyle is offline   Reply With Quote

Old   February 2, 2012, 15:04
Default
  #6
New Member
 
Paul Kirchner
Join Date: Dec 2011
Posts: 11
Rep Power: 5
pkirchner is on a distinguished road
Hello Kyle, I also feel like it may be the initial surface triangulation. When I run a surface repair, I get a 200+ pierced faces...on both initial surface, and on the remeshed representation. I created a new part for both the fan and sidepod..setting the fan to a 8"x8"x0.5" square. I followed the same procedure i was successful with when doing the radiator...(Remesher/Polyhedral) I also ran the thin mesher just incase. I've played around with manual surface repair...attempting to create the part from the fans curve on the boolean subtract. The mesh still doesnt coincide..using the thin mesher, and very fine mesh on both regions.
Attached Images
File Type: jpg SquareFanVolMesh.jpg (101.7 KB, 43 views)
File Type: jpg FanPiercedFaces.jpg (104.6 KB, 29 views)
pkirchner is offline   Reply With Quote

Old   February 2, 2012, 15:50
Default
  #7
Senior Member
 
Join Date: Mar 2009
Location: Austin, TX
Posts: 134
Rep Power: 9
kyle is on a distinguished road
Those intersections are supposed to be there on the initial input surface. That is your interface. You need to do a merge/imprint on those faces before you run the remesher. This will get rid of the surface check errors and merge the two surfaces that make up the conformal interface into one surface. Never run the remesher with intersecting, open, or non-manifold geometry.
kyle is offline   Reply With Quote

Old   February 2, 2012, 16:33
Default
  #8
New Member
 
Paul Kirchner
Join Date: Dec 2011
Posts: 11
Rep Power: 5
pkirchner is on a distinguished road
Yup, I understand it is the interface. I have no problem with the Inlet, and outlet face...it's just the sides of the face..the merge/imprint only finds a triangle pair about every 1/20th distance around it..the other surface does not contact the same boundary on the boolean region. I've got a meeting, but I'll play around with it a bit more tonight and let you know. Thanks for the speedy reply!
pkirchner 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] surface mesh merging problem everest ANSYS Meshing & Geometry 39 June 5, 2013 19:02
Multi Region Meshing with sHM marango OpenFOAM Native Meshers: snappyHexMesh and Others 3 March 27, 2012 00:51
external flow with snappyHexMesh chelvistero OpenFOAM 11 January 15, 2010 20:43
Trimmed cell and embedded refinement mesh conversion issues michele OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 2 July 15, 2005 04:15
Import gmsh msh to Foam adorean Open Source Meshers: Gmsh, Netgen, CGNS, ... 24 April 27, 2005 08:19


All times are GMT -4. The time now is 13:16.