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   March 14, 2011, 13:17
Default
  #21
Member
 
Alberto Pellegrino
Join Date: Jan 2011
Posts: 32
Rep Power: 6
AlbertoP is on a distinguished road
Hi, thanks Simon.

Actually it is a 2D mesh.
I have just merged quad cells (inner mesh around airfoil) created by ICEM with tri cells (far field) created by ANSYS-mesh.

I checked the tri mesh (created in ANSYS-mesh and imported into ICEM) creating the Fluent mesh file, and it works, so the problem is in the merging operation (I followed your instructions above).

Any idea with 2D mesh please?

many thanks!
AlbertoP is offline   Reply With Quote

Old   March 14, 2011, 16:08
Default
  #22
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,661
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Have you done the mesh checks in ICEM CFD? Did you see any issues with the single or multiple edge checks?
PSYMN is offline   Reply With Quote

Old   March 18, 2011, 09:35
Default
  #23
cjz
New Member
 
Join Date: Feb 2010
Posts: 14
Rep Power: 7
cjz is on a distinguished road
Hello Simon,
I am attempting to use ICEM CFD to mesh a 3D wind turbine airfoil. My rotor geometry is complete and in ICEM CFD. What I'm looking for is a toehold on how to get started with ICEM CFD in 3D. I'd like to use triangles on airfoil surfaces and stack prism on top for boundary layer cells. From there tets to the extents of the domain with again triangles at the surface. I've spent a few weeks banging away at ICEM with limited success. Long story short, is there a decent tutorial on how to get started on meshing such a geometry?

Any help would be most appreciated.

CJZ
cjz is offline   Reply With Quote

Old   March 18, 2011, 12:07
Default
  #24
Member
 
Alberto Pellegrino
Join Date: Jan 2011
Posts: 32
Rep Power: 6
AlbertoP is on a distinguished road
Hi Simon,

yes, I got many many errors of all kinds!

In addition, this is not a good strategy, because it is not a quickly repeatable operation if I need to modify something.

So, I want to change, and stay only on ICEM. So, could you please tell me how to get a tri-mesh around a quad-mesh, matching them? And is possible to have a tri-mesh on more surfaces to better control the growth rate, all matched?

Do you reckon it is a good strategy?

many thanks!
AlbertoP is offline   Reply With Quote

Old   March 21, 2011, 10:05
Default
  #25
Member
 
Alberto Pellegrino
Join Date: Jan 2011
Posts: 32
Rep Power: 6
AlbertoP is on a distinguished road
Simon,

got it, no problem, no need a reply...

Thanks again!
AlbertoP is offline   Reply With Quote

Old   March 25, 2011, 13:00
Default
  #26
Member
 
Alberto Pellegrino
Join Date: Jan 2011
Posts: 32
Rep Power: 6
AlbertoP is on a distinguished road
Sorry Simon,

I changed idea again.

Is that possible to mesh with blocking (quad) like you did in your video tutorial (airfoil 2d), and then attach around a tri mesh for the farfield? All in ICEM of course.

I created 5 surfaces around the inner surface containing the airfoil (quad mesh) but I can't figure out how to tell ICEM to "start" creating tri mesh from the border nodes of the quad mesh.

Hope I explained well...

Many thanks!

Alberto
AlbertoP is offline   Reply With Quote

Old   March 25, 2011, 13:01
Default
  #27
Member
 
Alberto Pellegrino
Join Date: Jan 2011
Posts: 32
Rep Power: 6
AlbertoP is on a distinguished road
...I mean if is possible to avoid to create quad and tri mesh not matching..so then avoiding to editing mesh..create hole..create loop..repair mesh (procedure you told me before).


Many thanks!

Alberto
AlbertoP is offline   Reply With Quote

Old   March 25, 2011, 18:17
Default respect line elements...
  #28
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,661
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Yes, it is possible... Mesh the hexa (quad) section first. Take care to associate the perimeter edges to curves that bound that section of the model. This will ensure that line elements form.

Then change the Surface meshing type to "Patch Conforming" "Tri". Make sure to turn on the global shell meshing parameters option for "respect line elements", this will make sure that the new mesh uses the line elements around the hexa as a base (instead of the curve sizes set on those curves).

While the blocking based quad mesh is loaded, go into Mesh => Create mesh => Surface Mesh Only...

Change the Input to "From Screen" and select the surfaces around your hex meshed surfaces...

Compute.

This should then mesh just those surrounding surfaces with patch conforming triangles using the line elements around the existing mesh as seeds.

Warning, this assumes the geometry is connected... If you build topology (or color by count), the curves between the surfaces should be red. You will also need to set reasonable sizes for the curves on the outside of the surfaces so they can mesh properly...
PSYMN is offline   Reply With Quote

Old   March 31, 2011, 18:58
Default
  #29
Member
 
Alberto Pellegrino
Join Date: Jan 2011
Posts: 32
Rep Power: 6
AlbertoP is on a distinguished road
Hi Simon,

thanks, got it, and it works. BUT...not well... I mean, the patch conforming is done, but in the part of the curve where the node density is very high, ICEM generates "bad" triangles (long and thin) instead of little uniform ones. In the final mesh there are no errors, so it's good to import into FLUENT, but I reckon it's not good in some areas from a generation point of view.

Any ideas please? Maybe the tool is strong but not enough for a patch conforming on a single curve where the distance between nodes is very different along it?

Another question, about my previous problem. I got a matching between two different mesh (created at different moments) editing them...deleting some cells...creating the loop...remeshing to fill the hole. But as per my previous posts, I got problems importing the mesh into FLUENT. Checking the mesh, I got errors like DUPLICATE ELEMENTS (I fixed them) and MISSING INTERNAL FACES (I fixed them as well). The problem is that some elements edges (the ones for whose I had duplicate and missing internal errors) appear as WALL into FLUENT, and they can not be change into INTERIOR.

Any suggestion also for that, please?

Many thanks for your patience!
Kind regards
AlbertoP is offline   Reply With Quote

Old   April 2, 2011, 10:23
Default
  #30
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,661
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Some pictures would help...

The long thin triangles problem sounds like your sizes jumped to far and it just connected the nodes on the perimeter of the loop (a fail safe). Are there any nodes on the interior of that surface? You may need to put a smaller size on some of the other sides so it can transition reasonably.

I don't have enough info to guess at your second question.
__________________
-----------------------------------------
Please help guide development at ANSYS by filling in these surveys

Public ANSYS ICEM CFD Users Survey

This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)...

CFD Online Users Survey
PSYMN is offline   Reply With Quote

Old   April 5, 2011, 18:53
Default
  #31
Member
 
Alberto Pellegrino
Join Date: Jan 2011
Posts: 32
Rep Power: 6
AlbertoP is on a distinguished road
OK, here's some pictures...

The first three well show you the problem... The fourth one shows you how I would like to get the cells growing (made in another way of course)... whereas the fifth one shows you how I got, I mean with patch dependent I am not able to get the cells growing even if I set curve parameters (like I did in another contest with success).

ps: about my second question...well...I don't know how to better explain... but no matter, I would be happy to solve the first problem.

Many thanks again!
Alberto

http://img828.imageshack.us/i/patchdependent3.png/
http://img204.imageshack.us/i/patchdependent2.png/
http://img807.imageshack.us/i/patchdependent1.png/
http://img141.imageshack.us/i/rightgrowing.png/
http://img269.imageshack.us/i/badgrowing.png/
AlbertoP is offline   Reply With Quote

Old   April 5, 2011, 20:35
Default
  #32
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,661
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
If you want it to be all triangles, you can set the type to "all tri", in the first few pics, the mesher is just trying its best to connect large triangles to small quads... the only way to do it better is to re-mesh the area including a few more cells on either side so the mesher can have some room to adjust sizes...
__________________
-----------------------------------------
Please help guide development at ANSYS by filling in these surveys

Public ANSYS ICEM CFD Users Survey

This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)...

CFD Online Users Survey
PSYMN is offline   Reply With Quote

Old   April 7, 2011, 18:24
Default
  #33
Member
 
Alberto Pellegrino
Join Date: Jan 2011
Posts: 32
Rep Power: 6
AlbertoP is on a distinguished road
Hi Simon,

OK, thanks. I figured out that is better to manually do the "matching operations".

About that, just one last question please: since it is a 2D configuration, of course I get single-edges around the perimeters and I "ignore" that.

But I can't understand why I get some single-edges also in a not perimetrical aera. Please see the image to understand where the problem is. (I created a hole around the quad-mesh and then did a re-mesh to get a match between quad-mesh and tri-mesh).

This single-edge problem is only there (and at his opposite corner, below). It is not a real problem to get good results in terms of lift and drag coefficients, but there is an interference in the wake, since FLUENT can not see these edges as interior, but rather as WALL...so the flow impacts on them creating two wakes that are not supposed to be.

Many thanks for your always quick replies!

http://img217.imageshack.us/i/singleedge.png/
AlbertoP is offline   Reply With Quote

Old   April 7, 2011, 20:32
Default Merge nodes.
  #34
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,661
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
There must be a topology (geometry) disconnect... You could prevent it with a build topology operation before meshing...

But you can also fix it easily. Go to Edit Mesh => merge Mesh => Merge nodes (with a tolerance). Put in a very small tolerance and select all the elements or the single edge subset, or you could just select the patches where these problems are...

It will merge nodes with their neighbors and the single edges will go away.
__________________
-----------------------------------------
Please help guide development at ANSYS by filling in these surveys

Public ANSYS ICEM CFD Users Survey

This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)...

CFD Online Users Survey
PSYMN is offline   Reply With Quote

Old   April 12, 2011, 06:51
Default
  #35
Member
 
Alberto Pellegrino
Join Date: Jan 2011
Posts: 32
Rep Power: 6
AlbertoP is on a distinguished road
OK Simon,
thank you very much for your invaluable support.

Kind regards

Alberto
AlbertoP is offline   Reply With Quote

Old   May 24, 2011, 12:29
Default
  #36
Member
 
Alberto Pellegrino
Join Date: Jan 2011
Posts: 32
Rep Power: 6
AlbertoP is on a distinguished road
Hi Simon,

about meshinq with patch conforming between quad and tri mesh... with "respect line elements"... what does it mean if after the mesh computing the inner quad mesh disappear? And only the outer tri mesh (just computed) remains.

Always better doing it manually? Or do know what the problem could be?
Many thanks

Alberto
AlbertoP is offline   Reply With Quote

Old   May 24, 2011, 13:05
Default
  #37
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,661
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
The new mesh shouldn't replace the original mesh, it should merge with it...

Off the top of my head, I am not sure where things went wrong for you.
__________________
-----------------------------------------
Please help guide development at ANSYS by filling in these surveys

Public ANSYS ICEM CFD Users Survey

This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)...

CFD Online Users Survey
PSYMN is offline   Reply With Quote

Old   March 6, 2013, 02:17
Default
  #38
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,904
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Quote:
Originally Posted by PSYMN View Post
As a teaser, here are some pics... The total mesh time from geometry to solver was about 15 or 20 minutes.
Simon this post was written in 2010. But I see the technology (multi-zone) used in these pics was made available in ICEM 14.5!!! Did you make this meshing when multi-zone was in testing phase ?
Far is offline   Reply With Quote

Old   March 6, 2013, 17:47
Default
  #39
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,661
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Quote:
Originally Posted by Far View Post
Simon this post was written in 2010. But I see the technology (multi-zone) used in these pics was made available in ICEM 14.5!!! Did you make this meshing when multi-zone was in testing phase ?
I may have posted those shortly before release, but I think it was with version 13 or what ever version we released that year... 14.5 was not the first release to include MultiZone, but it probably did include several man years of enhancements including hooking up Gambit sizing functions and TGrid Tetra. Work on MultiZone continues at a high pace, but work has focused on internal flow and FEA use cases.
__________________
-----------------------------------------
Please help guide development at ANSYS by filling in these surveys

Public ANSYS ICEM CFD Users Survey

This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)...

CFD Online Users Survey
PSYMN is offline   Reply With Quote

Old   June 5, 2013, 19:02
Default
  #40
Senior Member
 
Astio Lamar
Join Date: May 2012
Location: Pipe
Posts: 154
Rep Power: 5
asal is on a distinguished road
Hello

I have the problem exactly same as #1 fig 4, over the cut plane. this gonna happen when I want to use Delaunay meshing. there is problem with the Octree!
does anybody known what is the problem as well as the solution?
thanks.
asal 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 15:18.