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

Trimmer mesh problems - solution diverging

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

Like Tree1Likes
  • 1 Post By ashokac7

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   August 6, 2018, 17:36
Default Trimmer mesh problems - solution diverging
  #1
New Member
 
Ga
Join Date: Jul 2018
Posts: 16
Rep Power: 4
lightning0 is on a distinguished road
Hi,

I have an issue when using the trimmer mesh for an vehicle in wind tunnel simulation. When using the polyhedral mesh the volume mesh works fine and the solution converges but the mesh takes too long to generate. I used volumetric control regions around the vehicle and set the surface size to be 1 - 3 mm at the wheels and 10 - 12mm on the vehicle. The vehicle is 3m long. I tried using the surface wrapper but the vehicle disappears from the volume mesh, I don't understand why that occurs? I did run a surface repair on the surface mesh and it said zero problems.

Attached is the volume mesh

Thanks


lightning0 is offline   Reply With Quote

Old   August 7, 2018, 02:51
Smile
  #2
Senior Member
 
Ashok Chaudhari
Join Date: Aug 2016
Location: Pune, India
Posts: 243
Rep Power: 7
ashokac7 is on a distinguished road
Send a message via Skype™ to ashokac7
It looks like the problem with the quality of mesh. I prefer using polyhedral mesh for flow with complex geometries. Even if meshing time is large for poly-mesh, the quality of mesh is formed is better than trimmer (Hex). We even get less mesh count with poly.



There are some studies which even suggest that solution converges early with poly mesh set ups. Only problem is that for large geometries mesh count is very large, unlike trimmer which left the hanging node during growing mesh inside volume, so mesh count is far less.


Post the error message which you are getting. Right click on region and search for invalid cells with stringent criteria, like 1e-4 for volume change and 1e-5 for cell quality. Even check for skewness greater than 100. If there are cell below this criteria then search the region where these cell are appearing and do some mesh size change there.


Hope this helps.
ashokac7 is offline   Reply With Quote

Old   August 7, 2018, 11:54
Default
  #3
Member
 
André Pinto
Join Date: Oct 2017
Posts: 81
Rep Power: 4
AndreP is on a distinguished road
First make sure you have a quality mesh. Check the help files for "Mesh Quality" which should be available here:

file:///C:/Program%20Files/CD-adapco/12.04.010-R8/STAR-CCM+12.04.010-R8/doc/en/online/index.html#page/STARCCMP/GUID-FAB6B0AA-44A6-4A7B-AA27-A2EC92918B8F=en=.html#wwID0EJYW6

If not, just type "Mesh quality" in the help search.

Then, to check each, just plot a scalar plot, selecting each:

Face Validity: Below 1.0 is bad.
Cell Quality: Below 1e-5 is bad
Volume Change: Below: 0.01 is bad
Skewness Angle: Above 85 is bad
Chevron Quality Indicator: cells marked 1.0 are bad
Least Squares Quality: Less than 1e-3 is bad
Cell Warpage: Less than 0.15 is bad

After checking this you'll be able to see problematic areas, if you have some. Just need to refine them!

After ensuring there's a good mesh quality, it's just refining turbulent zones (Wake, or zones around big geometry changes) and then making sure your physics and turbulence models are the correct ones! I see from your image, that you don't seem to have Wake Refinement! You should!
AndreP is offline   Reply With Quote

Old   August 7, 2018, 12:28
Default
  #4
New Member
 
Ga
Join Date: Jul 2018
Posts: 16
Rep Power: 4
lightning0 is on a distinguished road
Thanks for the answers. I forgot to add to the initial post that when refining the mesh to around 1mm base size I would get an error when initializing the solution stating the x amount of cells have zero volume. Removing those invalid cells screwed up with my geometry as the residuals were diverging. I managed to solve the mesh issues by using the surface wrapper. I could refine the mesh and run the analysis with no issues.
lightning0 is offline   Reply With Quote

Old   August 8, 2018, 01:12
Default
  #5
Senior Member
 
Join Date: Nov 2010
Location: USA
Posts: 1,229
Rep Power: 20
me3840 is on a distinguished road
If your domain has a lot of negative volume cells you should not just remove them and keep going. This represents a fundamental problem with your meshing strategy, it should be explored, identified, and remeshed. For a simple geometry like this there's no reason to have negative volume cells.

The circles you see on your surface may be due to excessive prism collapsing. I would look at your prism mesh.
me3840 is offline   Reply With Quote

Old   August 8, 2018, 01:22
Smile
  #6
Senior Member
 
Ashok Chaudhari
Join Date: Aug 2016
Location: Pune, India
Posts: 243
Rep Power: 7
ashokac7 is on a distinguished road
Send a message via Skype™ to ashokac7
Zero or negative volume cells are not acceptable. Don't just delete them, you have to mesh with better strategy. Before moving on to solution, it is better to spend quite a bit of time on meshing. I heard this a lot of time at workplace, like a good analyst spend a lot of time on mesh. I don't want to do entire thing just because mesh was not adequate enough. Isn't it?
tisa likes this.
ashokac7 is offline   Reply With Quote

Old   August 8, 2018, 03:06
Default
  #7
New Member
 
Ga
Join Date: Jul 2018
Posts: 16
Rep Power: 4
lightning0 is on a distinguished road
Quote:
Originally Posted by me3840 View Post
If your domain has a lot of negative volume cells you should not just remove them and keep going. This represents a fundamental problem with your meshing strategy, it should be explored, identified, and remeshed. For a simple geometry like this there's no reason to have negative volume cells.

The circles you see on your surface may be due to excessive prism collapsing. I would look at your prism mesh.
By prism collapsing do you mean that I used too many prism layers which resulted in interference with each other? The solution converged fine after I used a smaller surface size and the surface wrapper with 20 prism layers at the surface. The circles on the geometry were also not present
lightning0 is offline   Reply With Quote

Old   August 8, 2018, 04:04
Default
  #8
Senior Member
 
Join Date: Mar 2009
Posts: 240
Rep Power: 14
Maddin is on a distinguished road
May you should try the CAD import, some CAD software has a bad maths behind the models and the exported models (STL) are showing the weakness of the software...

Sometimes it's better to use an external software for mesh generating. MeshLab as first step should help you a little bit.

Show us the remeshed surface and the imported surface for better help.
Maddin is offline   Reply With Quote

Old   August 8, 2018, 06:36
Default
  #9
New Member
 
Ga
Join Date: Jul 2018
Posts: 16
Rep Power: 4
lightning0 is on a distinguished road
The remeshed surface with the surface wraper is shown below. The initial surface is in the first post. The circles on the mesh are only present around the wheel arches now. I did get convergence with this mesh.

I imported the mesh in .igs format. The body was created in Alias and exported in .igs. The wheels were created in solidworks along with the entire assembly. Should I import the .sldasm file instead?

Thanks
I have meshlab installed. What operation would you recommend me performing?

Last edited by lightning0; August 8, 2018 at 08:08.
lightning0 is offline   Reply With Quote

Old   August 8, 2018, 07:58
Default
  #10
New Member
 
Owen
Join Date: Aug 2018
Posts: 20
Rep Power: 4
SoAero is on a distinguished road
My recommendation would be to identify where the poor quality cells are and then add custom controls to refine the surface/volume where required. This will do two things: 1) address your messing problems, 2) reduce the size of your mesh needed to run the simulation. Your geometry is very straightforward and you’re only doing one type of physics. You shouldn’t need a huge mesh.

Usually, the procedure is: fine wrap to capture the shape/geometry, coarser remesh to improve quality of surface, trim with volume controls where needed.

The cad you have is probably fine unless it’s causing you to have poor quality cells somewhere. The wrapper is good about smoothing over those gaps and overlaps.

Last edited by SoAero; August 8, 2018 at 07:59. Reason: Spelling
SoAero is offline   Reply With Quote

Reply

Tags
cfd, mesh, star ccm+, vehicle aerodynamics

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
Diverging solution for hypersonic flow lipiroy SU2 1 July 2, 2018 12:04
sliding mesh problem in CFX Saima CFX 45 September 22, 2015 10:53
Airfoil simulation solution interfered by mesh Dvergr OpenFOAM Running, Solving & CFD 1 September 28, 2014 02:05
[Commercial meshers] Several problems with the mesh conversion utility when converting the meshes from Gridgen su_junwei OpenFOAM Meshing & Mesh Conversion 2 July 26, 2008 23:58
fluent add additional zones for the mesh file SSL FLUENT 2 January 26, 2008 11:55


All times are GMT -4. The time now is 13:58.