CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Paraview & paraFoam

High Aspect Ratio Cells in Paraview

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

Like Tree4Likes
  • 4 Post By elisabet

Reply
 
LinkBack Thread Tools Display Modes
Old   April 7, 2011, 06:48
Default High Aspect Ratio Cells in Paraview
  #1
jms
Member
 
JosÚ
Join Date: Jan 2011
Posts: 73
Rep Power: 6
jms is on a distinguished road
Dear all,

Do any of you know how to check the cells with highest aspect ratio with Paraview? If there are cells with high aspect ratio checkMesh from OpenFOAM creates a file in "constant/sets" called "highAspectRatioCells". Is there any way to open this one in Paraview?

Thanks.

Regards,

JosÚ
jms is offline   Reply With Quote

Old   April 7, 2011, 10:31
Default
  #2
Member
 
Elisabet Mas de les Valls
Join Date: Mar 2009
Location: Barcelona, Spain
Posts: 61
Rep Power: 8
elisabet is on a distinguished road
Hi JosÚ,

Of course there is!

If you open your case with paraFoam, at the main page you see a list of options, among them:
-Update GUI
-Cache Mesh
-Extrapolate Walls
-Include Sets
-...
just click on 'Include Sets' and you'll see it.


If you prefer dealing with paraview, use the command:
foamToVTK -cellSet highAspectRatioCells
and load the file as usual.



enjoy!

elisabet
atg, gfoam, Alhasan and 1 others like this.
elisabet is offline   Reply With Quote

Old   April 7, 2011, 11:45
Default
  #3
jms
Member
 
JosÚ
Join Date: Jan 2011
Posts: 73
Rep Power: 6
jms is on a distinguished road
Thank you very much for your help!

What about this other thread I started in here?... do you know any thing?

GrÓcies!

JosÚ
jms is offline   Reply With Quote

Old   May 13, 2013, 03:52
Default
  #4
Member
 
Join Date: Aug 2011
Posts: 74
Rep Power: 5
idefix is on a distinguished road
Hello,

foamToVTK -cellSet highAspectRatioCells
is not working in my case.

I get the error massage:
--> FOAM FATAL ERROR:
Cannot find file "" in directory "polyMesh/sets" in times 0 down to constant

From function Time::findInstance(const fileName&, const word&, const IOobject::readOption, const word&)
in file db/Time/findInstance.C at line 140.

FOAM exiting

What is wrong? Can somebody help me?

Thanks a lot
idefix is offline   Reply With Quote

Old   May 14, 2013, 17:49
Default
  #5
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,301
Blog Entries: 34
Rep Power: 84
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Greetings idefix,

Did you run checkMesh? Did it report any high aspect ratio cells?

You might also want to try the full diagnosis, by running:
Code:
checkMesh -allGeometry -allTopology
Best regards,
Bruno
wyldckat is offline   Reply With Quote

Old   May 17, 2013, 02:03
Default
  #6
Member
 
Join Date: Aug 2011
Posts: 74
Rep Power: 5
idefix is on a distinguished road
Hello Bruno,

thanks for your help.

checkMesh that┤s that everything is ok

but checkMesh -allGeometry -allTopology

says:
Quote:

Cell determinant (wellposedness) : minimum: 0 average: 0
***Cells with small determinant found, number of cells: 4680
<<Writing 4680 under-determined cells to set underdeterminedCells
Concave cell check OK.

Failed 1 mesh checks.

End
It┤s a test case and therefore the grid is very small. It has only 4680 cells - so every cell is "damaged".

But what does it exactly mean?

Thanks a lot
Regards
Idefix
idefix is offline   Reply With Quote

Old   May 17, 2013, 02:34
Default
  #7
Member
 
Join Date: Aug 2011
Posts: 74
Rep Power: 5
idefix is on a distinguished road
Hello again,

I just try a little and was wondering about the error massage because the grid looks nice to me.

By accident the error massage disappeared when I add more cells in the third dimension.
Before the grid has only 1 cell in the third dimension.

Why is this command (foamToVTK -cellSet highAspectRatioCells) not working for a 2d grid?

Thanks a lot
Idefix
idefix is offline   Reply With Quote

Old   May 17, 2013, 18:14
Default
  #8
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,301
Blog Entries: 34
Rep Power: 84
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Hi Idefix,

You cannot get foamToVTK to process "highAspectRatioCells", simply because checkMesh did not find any cells with high aspect ratio.

What you could have done when you got the error for "under-determined cells", is use foamToVTK to give you a VTK file for the cellSet named "underdeterminedCells":
Code:
foamToVTK -cellSet underdeterminedCells
Only because you got this message:
Quote:
Code:
<<Writing 4680 under-determined cells to set underdeterminedCells
Best regards,
Bruno
wyldckat is offline   Reply With Quote

Old   February 11, 2014, 01:49
Default Check if all cells have an aspect ratio of 1?
  #9
Senior Member
 
Srivathsan N
Join Date: Jan 2013
Location: India
Posts: 101
Rep Power: 4
Sherlock_1812 is on a distinguished road
Hi all,

I have a mesh that checkMesh has certified to be OK. Maximum aspect ratio is reported as 1.9. I would like to confirm if this aspect ratio is not in my region of interest where i'd like all cells to have an aspect ratio close to 1.

So for a correct mesh, can I still view aspect ratio of all cells in paraView? And maybe plot the variation of aspect ratio along x-direction?
__________________
Regards,

Srivaths
Sherlock_1812 is offline   Reply With Quote

Old   February 16, 2014, 15:16
Default
  #10
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,301
Blog Entries: 34
Rep Power: 84
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Greetings Srivaths,

Although it would be very useful to get checkMesh to write out all of the fields calculated for mesh characteristics, unfortunately there isn't one in OpenFOAM by default, nor am I aware of any community source code utility that does this.

Nonetheless, if you're interested in creating such an utility, have a look into the method "Foam::primitiveMeshTools::cellClosedness": https://github.com/OpenFOAM/OpenFOAM...shTools.C#L217
By the way, Github has a nice feature of searching for code inside the repository, by using the search edit box on the top of the page, so it's easy to find out which methods are calling this one!

Best regards,
Bruno
wyldckat is offline   Reply With Quote

Old   February 17, 2014, 01:04
Default
  #11
Senior Member
 
Srivathsan N
Join Date: Jan 2013
Location: India
Posts: 101
Rep Power: 4
Sherlock_1812 is on a distinguished road
Thank you Bruno.
__________________
Regards,

Srivaths
Sherlock_1812 is offline   Reply With Quote

Old   September 3, 2014, 11:51
Default
  #12
New Member
 
miladrakhsha
Join Date: Aug 2012
Posts: 27
Rep Power: 4
miladrakhsha is on a distinguished road
Hi,
I am working with paraView 3.14.1 but seems like there is no include set option available. Any idea?

Also, is there anyway I can change the version of paraview that I want to open the case with ? I have two versions of paraView and I would like to use the older version for post-processing even when I am using the new version of OpenFOAM which is by default associated with the newer version of paraView.
miladrakhsha is offline   Reply With Quote

Old   September 13, 2014, 16:47
Default
  #13
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,301
Blog Entries: 34
Rep Power: 84
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Greetings miladrakhsha,

Regarding the first question, if you're using OpenFOAM 2.x:
Code:
paraFoam -builtin
If you're using foam-extend:
Code:
paraFoam -nativeReader
Regarding the second question, without knowing how exactly which versions of OpenFOAM you're using and which ParaView versions, the best answer I can come up quickly is to point you to this post: R.e openFoam 1.6 - post #2

Best regards,
Bruno
wyldckat 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
SnappyHexMesh for internal Flow vishwa OpenFOAM Native Meshers: snappyHexMesh and Others 23 August 6, 2014 03:50
external flow with snappyHexMesh chelvistero OpenFOAM 11 January 15, 2010 20:43
paraFoam reader for OpenFOAM 1.6 smart OpenFOAM Installation 13 November 16, 2009 22:41
High aspect ratio in viscous sublayer? Marius Main CFD Forum 0 December 22, 2005 09:15
Help Needed: High aspect ratio Michelle FLUENT 0 January 24, 2003 04:15


All times are GMT -4. The time now is 15:06.