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

[ICEM] surface mesh merging problem

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

Like Tree3Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   June 9, 2010, 11:31
Default surface mesh merging problem
  #1
New Member
 
Join Date: May 2010
Location: Tokyo, Japan
Posts: 6
Rep Power: 7
everest is on a distinguished road
Hi everybody,
I'm working on a project of simulating DLR-F4 wing-body configuration(half model)with CFX. The orginal unstructured mesh was generated with Octree method using ICEM-CFD. In order to save the number of grid points, I was considering making anisotropic mesh(large aspect ratio along spanwise) on the wing. Then I delteted all the volume mesh and the surface mesh on the wing, and got a structured surface mesh(quads) from some other guy. I intended to concatenate thses surface meshes at the wing body intersection and grow volume meshes from this new surface mesh with bottom-up methods within ICEM-CFD such as Delauney. Some problems occured during the process and I really need suggestions from experienced ICEM users.

1. tris + quads or tris + tris
Now I have triangle surface mesh on the fuselage, symmetry plane and farfiled. Should I directly connected the quds on the wing with tris on the fuselage or first split the quad mesh on the wing into tris? I was suggested converting the wing quad mesh into tris first. Can ICEM grow volume tetras and prisms if I have fuselage tris and wing quds sewn together?

2. surface mesh merging
After loading the geomety and surface mesh respectively, nodes on the wing and fuselage didn't match together at the intersection line. I finally found the "stitch edges" command useful which can make the mesh on both sides conformal. After sewing the surface mesh together, there were still some seemingly bad elements. Manual operatons such as merging and projecting were performed node by node. The whole process was a little tedious and sometimes difficult.

Can someone recommend general proceduals or better guidlines of merging and then fixing surface meshes? Are there convinient commands or operations in ICEM when joining two surface meshs.I could only find demos on volume mesh merging on ANSYS website.

btw, I have another question here. Due to their large aspect ratio, the wing tri mesh splitted from quad mesh seem to have low quality according to the ICEM quality criterion. Should I still have these surface meshes smoothed globally?

3. A weird volome mesh was grown from the sewn surface mesh

I finally elininated some obviously bad elements and went through the mesh checking procedure. Tetra volume meshes were grown using Delauney (with TGlib and and AF), but a fatal error occured. The tetra meshes grew out of my farfield boundary (the red lines in my last attached graphs). There seemed to be some unacceptable large tetras grown out. I really didn't know the reason.
Attached Images
File Type: jpg mesh before merging.jpg (66.8 KB, 739 views)
File Type: jpg stitch_LE.jpg (83.9 KB, 625 views)
File Type: jpg stitch_TE.jpg (51.5 KB, 567 views)
File Type: jpg 2.3.jpg (52.1 KB, 548 views)
zkdkeen likes this.
everest is offline   Reply With Quote

Old   June 10, 2010, 11:09
Default Quick Thoughts
  #2
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
1) You can stitch and grow delaunay tetra off quads or tri's. You can also grow prism of either, if you grow the prism first. If you do the delaunay first, you have more trouble because Prism has trouble moving pyramids.

2) Yes, this is not an ideal procedure. There are many faster ways to mesh this model in ICEM CFD. There is a actually a tutorial for bottom up (patch conforming) surface meshing on this F6 (to get higher aspect ratio elements), followed by delaunay and prism, but I don't like it. I think it is faster to do this model with ICEM CFD Hexa or MuliZone. The easiest way is Octree (which you already tried), but it is less efficient.

Perhaps your best option would be to import this wing mesh, then Edit Mesh => Repair => Build mesh topology so it would be properly associated to the geometry (surface and curve projected nodes). Convert the quads to tri's (optional) and then run Octree mesh with the option to keep the existing wing mesh. Then it will generate the octree mesh in accordance with the existing mesh and everything would be automatically connected. Then you could run delaunay to replace the octree volume mesh, etc. There would be hardly any interactive steps. You may have some issues with high aspect ratio mesh along the wing not conforming properly and need to repair a little bit here or there.

Stitch edges is the primary tool for merging edge to edge surface mesh. You would then check for single edges and use a combination of "split edges" and "merge nodes" to clean up any left overs. It is tedious, so I only do it when absolutely necessary.

No, don't smooth this wing surface. These thin high aspect ratio elements do have low quality by all definitions and the smoother will try to fix them. You don't want that, so freeze them. There are several ways to do this, including that you can lock the nodes under Edit Mesh => Repair.


3) Not sure about your weird volume mesh. Did you run your mesh checks before generating that? You will want to make sure you have no overlapping elements or single edges in your model. Delaunay needs a good starting point to produce a good mesh. Garbage in, Garbage out.
PSYMN is offline   Reply With Quote

Old   June 10, 2010, 12:20
Default
  #3
New Member
 
Join Date: May 2010
Location: Tokyo, Japan
Posts: 6
Rep Power: 7
everest is on a distinguished road
Simmon, I really appreciate your suggestions. I'll try them ASAP and post new results here.

As for the weird volume mesh in the last picture, I once did mesh check and fix errors like dumplicating elements before growing tetra mesh. I might need recheck them carefully.
everest is offline   Reply With Quote

Old   June 12, 2010, 13:28
Default
  #4
New Member
 
Join Date: May 2010
Location: Tokyo, Japan
Posts: 6
Rep Power: 7
everest is on a distinguished road
After rechecking my combined surface mesh, I found two overlapping tri elements. Finally the surface mesh went through mesh quality checking (Fig. 1) . The volume tetra mesh was then successfully from surface mesh using Delauney (Fig. 2). When I tried to insert prism layer into volume tetras, something went wrong. The final iteration of prism generating kept on running for a rather long time, printing message like the following (Fig. 3).
final iteration: worst collapse time 0.318662 worst quality -1
worst vertex 23267 21365 23266
completed smoothing
really bad tet quality (8.49741e-006)
cur_verts[0] = 1010
cur_verts[1] = 106980
cur_verts[2] = 21664
cur_verts[3] = 1011
old_verts[0] = 1010
old_verts[1] = 106980
old_verts[2] = 21664
old_verts[3] = 1011
really bad tet quality (6.47109e-006)
cur_verts[0] = 105915
cur_verts[1] = 21596
cur_verts[2] = 726
cur_verts[3] = 21573
old_verts[0] = 105915
old_verts[1] = 21596
old_verts[2] = 726
...
...
I just know this may be due to bad tetra quality, but I don't know how to avoid them. Tetra mesh form the anisotropic wing tri mesh (especially in area such as trailling edge) seem to undoubtedly in low quality .

I had also tried to generate prism layer first and then volume tetras. Through some pyramids appeared, prism layer could be grown around the wing and fuselage (Fig. 4). The weired volume mesh came again when I growed volume mesh with existing surface mesh and prism layers using delauney (Fig. 5).
Attached Images
File Type: jpg 1.jpg (90.1 KB, 285 views)
File Type: jpg 2.jpg (93.9 KB, 308 views)
File Type: jpg 3.jpg (94.9 KB, 240 views)
File Type: jpg 4.jpg (88.5 KB, 206 views)
File Type: jpg 5.jpg (91.2 KB, 216 views)
everest is offline   Reply With Quote

Old   June 12, 2010, 19:46
Default
  #5
New Member
 
Join Date: May 2010
Location: Tokyo, Japan
Posts: 6
Rep Power: 7
everest is on a distinguished road
I'm going to freak out.

I tried to follow simmon's suggestion, keeping the existing wing surface mesh loaded; thereafter generated other mesh with octree method. Unfortunately, a warning box "Your geometry has a hole, do you want to repair it" popped out at final steps. You can see them in my pictures attached. There are holes near the trailling edge. I don't konw why the wing surface mesh are ruined with "Use Existing Mesh Parts" option toggled on. I sliced a plane to view the volume mesh, and discovered that the volume mesh even grown inner the wing. Perhaps this is the reason why holes appeared.

I first thought it was due to mesh smoothing, and checked off "Sooth mesh" option in volume meshing parameters. The holes with yellow curves stll exists.

I really cann't figure out the problem. There didn't exist any yellow curve in the geometry level, when I built the geometry topology. How did the wing volume mesh grow inward? Are there any options in ICEM that can totally freeze some part of the mesh?
Attached Images
File Type: jpg 1.jpg (95.4 KB, 171 views)
File Type: jpg 2.jpg (58.4 KB, 106 views)
File Type: jpg 3.jpg (88.3 KB, 100 views)
File Type: jpg 4.jpg (88.4 KB, 132 views)
everest is offline   Reply With Quote

Old   June 17, 2010, 12:32
Default
  #6
New Member
 
Join Date: May 2010
Location: Tokyo, Japan
Posts: 6
Rep Power: 7
everest is on a distinguished road
Perhaps I'm not on the right track of solving this problem. Volume mesh often goes wrong from the merged surface mesh.

I'd like to turn to the 'multizone' approach. I have no experience in blocking and growing structural meshes. Are there any tutorials or guidlines on 'multizone' method? Please let me konw.
everest is offline   Reply With Quote

Old   June 18, 2010, 09:32
Default Try
  #7
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
I will try to create and post a movie to MulitZone mesh this model... I have done it a number of times for various people, but not properly recorded it.
aruv and asal like this.
PSYMN is offline   Reply With Quote

Old   June 18, 2010, 10:29
Default Pics of F6 meshed with MultiZone.
  #8
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
As a teaser, here are some pics... The total mesh time from geometry to solver was about 15 or 20 minutes.
Attached Images
File Type: jpg F6_Preview5_0003_edges.jpg (81.1 KB, 496 views)
File Type: jpg F6_Preview5_0004_edges.jpg (97.8 KB, 455 views)
File Type: jpg F6_Preview5_0006_Under.jpg (93.1 KB, 379 views)
File Type: jpg F6_Preview5_0008_Zoom.jpg (77.4 KB, 379 views)
File Type: jpg F6_Preview5_007.jpg (63.8 KB, 337 views)
PSYMN is offline   Reply With Quote

Old   August 3, 2010, 10:07
Default
  #9
siw
Senior Member
 
Join Date: Jul 2009
Posts: 443
Rep Power: 13
siw will become famous soon enough
PSYMN, I hope your still going to make this movie (for the ANSYS youtube channel?). Is a Hexa licence required as well as a Tetra/Prism licence to make this MultiZone mesh?
siw is offline   Reply With Quote

Old   August 3, 2010, 17:36
Default MultiZone is considered ICEM CFD Hexa functionality.
  #10
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Nope, MultiZone just needs a Hexa license (aihexa) (or aienv key or aiaddon key or amesh_extended key). It does not require an aitetra key.

Not sure when I will have time... The summer is flying by.

Simon
PSYMN is offline   Reply With Quote

Old   September 4, 2010, 13:50
Default Better way f stitching two surface meshes
  #11
New Member
 
Dhananjay B. Deshmukh
Join Date: Jan 2010
Location: Pune, INDIA
Posts: 11
Rep Power: 7
dhananjay1287 is on a distinguished road
one can uses close hole feature of ICEM to stitch surface meshes
it works better than stitch edges option. also good transition can be achieved which will reduce manual wok later to improve quality.

I have explained the procedure in images.
images:
1)http://picasaweb.google.co.in/lh/pho...eat=directlink
2)http://picasaweb.google.co.in/lh/pho...eat=directlink
3)http://picasaweb.google.co.in/lh/pho...eat=directlink
4)http://picasaweb.google.co.in/lh/pho...eat=directlink
5)http://picasaweb.google.co.in/lh/pho...eat=directlink
6)http://picasaweb.google.co.in/lh/pho...eat=directlink

sorry i dont know how to atach images in reply

hope this is helpful !!!!
dhananjay1287 is offline   Reply With Quote

Old   September 4, 2010, 14:05
Default here are the images attached
  #12
New Member
 
Dhananjay B. Deshmukh
Join Date: Jan 2010
Location: Pune, INDIA
Posts: 11
Rep Power: 7
dhananjay1287 is on a distinguished road
here are the files
Attached Images
File Type: jpg merege shell mesh 01.jpg (102.0 KB, 390 views)
File Type: jpg merege shell mesh 02.jpg (102.2 KB, 327 views)
File Type: jpg merege shell mesh 03.jpg (102.7 KB, 307 views)
File Type: jpg merege shell mesh 04.jpg (98.8 KB, 295 views)
File Type: jpg merege shell mesh 05.jpg (102.8 KB, 300 views)
dhananjay1287 is offline   Reply With Quote

Old   September 4, 2010, 14:07
Default
  #13
New Member
 
Dhananjay B. Deshmukh
Join Date: Jan 2010
Location: Pune, INDIA
Posts: 11
Rep Power: 7
dhananjay1287 is on a distinguished road
sorry, here is the last file
Attached Images
File Type: jpg merege shell mesh 06.jpg (104.7 KB, 258 views)
dhananjay1287 is offline   Reply With Quote

Old   February 24, 2011, 15:06
Default
  #14
Member
 
Alberto Pellegrino
Join Date: Jan 2011
Posts: 32
Rep Power: 6
AlbertoP is on a distinguished road
Quote:
Originally Posted by dhananjay1287 View Post
here are the files
Hi Dhananjay,

I need to do a similar thing (matching 2 different surface mesh, one quad and one tri): please could you kindly better explain how to do the steps you attached above?

I am ok until figure 3, but I am not able to do the 4th and 5th step.

Many thanks, very helpful!

best regards,

Alberto
AlbertoP is offline   Reply With Quote

Old   February 25, 2011, 03:51
Default
  #15
New Member
 
Dhananjay B. Deshmukh
Join Date: Jan 2010
Location: Pune, INDIA
Posts: 11
Rep Power: 7
dhananjay1287 is on a distinguished road
ICEM mesh repair tool needs to find hole in your mesh to fill that hole.
In order to use that oration to join surface meshes you have to fool the ICEM in thinking there is hole in the surface mesh. To create that you need to merge end nodes, so that when you repair the mesh ICEM can find the close loop which then can be filled with tri mesh.
dhananjay1287 is offline   Reply With Quote

Old   February 25, 2011, 19:42
Default
  #16
Member
 
Alberto Pellegrino
Join Date: Jan 2011
Posts: 32
Rep Power: 6
AlbertoP is on a distinguished road
Thanks for your quick reply.

I understood this concept, but I asked you if you could explain how to merge end nodes and to do the close loop. I mean, some pratical clues/hints/indications about ICEM commands.

I now it is annoying, but please I need to do that in a very short time.

It is a little quad-mesh around an airfoil merged with a farfield tri-mesh; I deleted some tri-cells around the quad-mesh to create the hole, but can't figure out how to merge end nodes to create the close loop.

Many thanks again for your availability.
Kind regards,

Alberto
AlbertoP is offline   Reply With Quote

Old   February 26, 2011, 07:54
Default
  #17
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Edit mesh => Merge => Merge nodes...

You just need to close the sides, you could even Edit mesh => Create a few tri elements. If you create them from nodes, they will already be merged.

Tip, when you do go to close the hole, the first element edge you select (before hitting "l" to select all the neighbors) will determine the part name of the final fill mesh.
PSYMN is offline   Reply With Quote

Old   March 10, 2011, 07:54
Default
  #18
Member
 
Alberto Pellegrino
Join Date: Jan 2011
Posts: 32
Rep Power: 6
AlbertoP is on a distinguished road
Thanks Dhananjay and Simon,

I got it... I am not able to create the right loop hitting "l", but selecting all edges manually it works.

If someone has the same problem maybe is useful to know that sometimes it is required to refine mesh close to the hole, in case of big difference of cells dimension between the two mesh to match. That was my problem, could not make it work without a refinement.

Great, many thanks again.
AlbertoP is offline   Reply With Quote

Old   March 11, 2011, 14:13
Default
  #19
Member
 
Alberto Pellegrino
Join Date: Jan 2011
Posts: 32
Rep Power: 6
AlbertoP is on a distinguished road
I correct myself:

able to get the loop hitting "l", so great, got my hybrid mesh.

But now, a problem: when I go to create the Fluent mesh file, I get some errors like "face (near node xxx) is attached to more than 2 cells ... error in computing cell connectivity ... child process exited abnormally".

Any idea, please?

Many thanks!

Alberto
AlbertoP is offline   Reply With Quote

Old   March 12, 2011, 18:46
Default
  #20
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Usually, you have shells (face elements) around a fluid volume... So you would have one cell attached to each face.

If you had faces between two volumes, then each face would have 2 cells attached. That is the most you should have.

In your case, it says you have more than 2 cells... Have you generated overlapping volume mesh? (not replaced when you regenerated?)

Run a cut plane thru the model and check for this. Actually, run thru the mesh checks and you should get several violations. You should always run the checks before exporting to the solver anyway...
PSYMN 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] Unstructure Meshing Around Imported Plot3D Structured Mesh ICEM kawamatt2 ANSYS Meshing & Geometry 17 December 20, 2011 12:45
[ICEM] [Student] Problem: Nodes Merging FALCON_SR71 ANSYS Meshing & Geometry 8 March 21, 2010 06:47
how to extend FSI 2D codes to 3D, need advises abouziar Main CFD Forum 1 May 30, 2008 04:08
Icemcfd 11: Loss of mesh from surface mesh option? Joe CFX 2 March 26, 2007 18:10
CFX4.3 -build analysis form Chie Min CFX 5 July 12, 2001 23:19


All times are GMT -4. The time now is 20:56.