CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Pointwise & Gridgen

Checking the quality of the meshing

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

Reply
 
LinkBack Thread Tools Display Modes
Old   June 1, 2013, 07:43
Default Checking the quality of the meshing
  #1
Member
 
Join Date: Nov 2012
Posts: 62
Rep Power: 4
Naruto is on a distinguished road
Dear pointwise users,
Hello everyone. I have lots of questions in my mind regarding this issue. I am posting in points.

# I am currently using OpenFOAM as solver and pointwise as meshing utility. I think OpenFOAM is very sensitive about two issues. They are: Orthogonality and Skewness. Recently I have made a mesh and checked the skewness in pointwise using centroid skewness and equiangle skewness options. In both cases pointwise showed reasonable values like <1. But in OpenFOAM when I tried using checkMesh command I found out skewness of around 70.

I know that the definition of skewness may vary from software to software. Could anyone give me a hint of checking the skewness of meshing in pointwise in such a way which would give me compatible values to OpenFOAM?

# This query is not solely related to pointwise. My question is how could I decrease skewness and keep orthogonality while meshing in pointwise? Some points are like maintaining good aspect ratio and high induced angle.

My question is could you please tell me a certain range of values? Like right now I am preparing a mesh and in one 2-D plane I am finding a minumum induced angle of 18 degree. Is it a reasonable value? The plane is along the flow direction.

Thanks for your time.
Naruto is offline   Reply With Quote

Old   June 1, 2013, 17:26
Default
  #2
Senior Member
 
Chris Sideroff
Join Date: Mar 2009
Location: Ottawa, ON, CAN
Posts: 368
Rep Power: 12
cnsidero is on a distinguished road
Yes there is a bit of a disconnect between the available examine metrics in Pointwise and what OpenFOAM checks for. One reason being some of OpenFOAM's metrics use face information and Pointwise does not store faces - it only stores points and cells - thus it can't compute a face-based metric.

Pointwise's metrics are all defined in Sec. 6.6 of the User Manual. You can access it through the Help menu.

As for OpenFOAM's, you have to dig a little in the source code to figure what they are. OpenFOAM's skewness is a measure of the deviation of the vector connecting the two cell centers adjacent to a face and the mid-point of that face. OpenFOAM also checks for orthogonality which it defines to be the deviation angle between the adjacent cell centers vector and the face normal. Lastly OpenFOAM checks for aspect ratio which has the same definition as Pointwise (and most other meshers and solvers).

Your last question is a bit vague as mesh quality tends to be application and mesh specific. But in general, I will say use structured meshing for problems where you can and use hybrid (prisms near walls, tets elsewhere) meshing for more complex problems.

If you can show me example, I can give you some more specific guidance about what to look for and ranges of acceptable values.

-Chris

Quote:
Originally Posted by Naruto View Post
Dear pointwise users,
Hello everyone. I have lots of questions in my mind regarding this issue. I am posting in points.

# I am currently using OpenFOAM as solver and pointwise as meshing utility. I think OpenFOAM is very sensitive about two issues. They are: Orthogonality and Skewness. Recently I have made a mesh and checked the skewness in pointwise using centroid skewness and equiangle skewness options. In both cases pointwise showed reasonable values like <1. But in OpenFOAM when I tried using checkMesh command I found out skewness of around 70.

I know that the definition of skewness may vary from software to software. Could anyone give me a hint of checking the skewness of meshing in pointwise in such a way which would give me compatible values to OpenFOAM?

# This query is not solely related to pointwise. My question is how could I decrease skewness and keep orthogonality while meshing in pointwise? Some points are like maintaining good aspect ratio and high induced angle.

My question is could you please tell me a certain range of values? Like right now I am preparing a mesh and in one 2-D plane I am finding a minumum induced angle of 18 degree. Is it a reasonable value? The plane is along the flow direction.

Thanks for your time.
cnsidero is offline   Reply With Quote

Old   June 2, 2013, 08:18
Default
  #3
Member
 
Join Date: Nov 2012
Posts: 62
Rep Power: 4
Naruto is on a distinguished road
Thanks for your reply. Okay here is what I want to do. Right now I just want to simulate a VAWT consisting of only three blades. Yes the geometry will be of only three straight blades. I want a rough simulation. I am doing this only to check my understanding of 3-D meshing. Here is my starting geometry.Forum.jpg

As you can see it is a fraction (1/3 to be precise) of a circular cylinder. I want to mesh it and copy the mesh twice in 120 degree interval to complete my circular cylindrical domain.

Now comes the problem. As I have told you earlier I want the simulation to be very rough and less time consuming. So I am trying to keep no. of cells as low as possible. My blade has very high aspect ratio. The chord length is only 2.2m and the span length is 85m. Span wise I have divided the connector in only 13 points. As a result when I create surface mesh and extrude it I could see high aspect ratio. Forum_1.jpg

Could you give me hints of effective meshing with low no. of cells?
Thanks for your time
Naruto is offline   Reply With Quote

Old   June 3, 2013, 09:39
Default
  #4
Senior Member
 
Chris Sideroff
Join Date: Mar 2009
Location: Ottawa, ON, CAN
Posts: 368
Rep Power: 12
cnsidero is on a distinguished road
Naruto,

My suggestion for this case would be to make an all structured mesh. Furthermore, since your blade [appears] to not have any twist or sweep I would create a 2D mesh of the sector cross section then create an extrusion in the axial direction. For the axial extrusion it is possible for use a non-uniform spacing through a user specified distribution.

Regarding your concern about aspect ratio. Having a high aspect ratio in general isn't a bad thing provided the gradients are too steep in the coarse direction. I've seen good solutions from OpenFOAM on meshes with aspect ratio over 10,000. In your case it's perfectly OK to have a coarse spacing along the blade (and have an aspect ratio of 500-1000) as there won't be much flow variation along the blade. Only near the ends of the blades where you'll get the induced vortex.

If you're still stuck let me know. If I have some time, I'll throw together I a quick example demo'ing my suggestions.

-Chris

Quote:
Originally Posted by Naruto View Post
Thanks for your reply. Okay here is what I want to do. Right now I just want to simulate a VAWT consisting of only three blades. Yes the geometry will be of only three straight blades. I want a rough simulation. I am doing this only to check my understanding of 3-D meshing. Here is my starting geometry.Attachment 22318

As you can see it is a fraction (1/3 to be precise) of a circular cylinder. I want to mesh it and copy the mesh twice in 120 degree interval to complete my circular cylindrical domain.

Now comes the problem. As I have told you earlier I want the simulation to be very rough and less time consuming. So I am trying to keep no. of cells as low as possible. My blade has very high aspect ratio. The chord length is only 2.2m and the span length is 85m. Span wise I have divided the connector in only 13 points. As a result when I create surface mesh and extrude it I could see high aspect ratio. Attachment 22319

Could you give me hints of effective meshing with low no. of cells?
Thanks for your time
cnsidero is offline   Reply With Quote

Reply

Tags
openfoam, quality check

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
critical error during installation of openfoam Fabio88 OpenFOAM Installation 21 June 2, 2010 03:01
Problems in compiling paraview in Suse 10.3 platform chiven OpenFOAM Installation 3 December 1, 2009 08:21
OpenFOAM installation problem on Linux 32bit kumar OpenFOAM Installation 0 April 27, 2007 05:41
Help%7e%7einstall openfoam13 on fc5%7e%7e aderliner OpenFOAM Installation 2 September 11, 2006 07:24
Gerris software installation mer Main CFD Forum 2 November 12, 2005 09:50


All times are GMT -4. The time now is 01:07.