CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Meshing & Mesh Conversion

[Commercial meshers] ideasUnvToFoam Cell type not supported

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

Like Tree11Likes
  • 1 Post By alinuman15
  • 2 Post By wyldckat
  • 2 Post By alinuman15
  • 3 Post By alinuman15
  • 2 Post By wildemam
  • 1 Post By Sachin m

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   July 16, 2017, 01:16
Default ideasUnvToFoam Cell type not supported
  #1
Member
 
Ali Noaman Ibrahim
Join Date: Sep 2015
Location: US_Chicago
Posts: 97
Rep Power: 10
alinuman15 is on a distinguished road
Dear All:-
I used Salome V8_2_0 to generate successfully NETGEN 1D-2D-3D mesh grouped on geometry. However, when used ideasUnvToFoam utility I got the following error:-
Code:
Create time

Processing tag:164
Starting reading units at line 3.
l:1
units:"  SI: Meter (newton)"
unitType:2
Unit factors:
    Length scale       : 1
    Force scale        : 1
    Temperature scale  : 1
    Temperature offset : 273.15


Processing tag:2420
Skipping tag 2420 on line 9
Skipping section at line 9.

Processing tag:2411
Starting reading points at line 20.
Read 3873594 points.

Processing tag:2412
Starting reading cells at line 7747211.
First occurrence of element type 22 for cell 1 at line 7747212
--> FOAM Warning : 
    From function readCells(IFstream&, label&)
    in file ideasUnvToFoam.C at line 467
    Reading "Mesh_1.unv" at line 7747212
    Cell type 22 not supported


--> FOAM FATAL IO ERROR: 
Attempt to get back from bad stream

file: IStringStream.sourceFile at line 0.

    From function void Istream::getBack(token&)
    in file db/IOstreams/IOstreams/Istream.C at line 56.

FOAM exiting
Any suggesstion ?
Thank you in advance

Last edited by wyldckat; August 27, 2017 at 10:27. Reason: Added [CODE][/CODE] markers
alinuman15 is offline   Reply With Quote

Old   July 17, 2017, 13:44
Smile
  #2
Member
 
Ali Noaman Ibrahim
Join Date: Sep 2015
Location: US_Chicago
Posts: 97
Rep Power: 10
alinuman15 is on a distinguished road
Dear mattijs:-
I have produced 3D (2D-3D NETGEN) mesh by Salome V_8.2.0 and exported it to OpenFoam2.4.0. However, I got the error shown in the inserted image. From your old suggestion about similar case I knew that the solution is to find a newer version of the file ideasUnvToFoam.C in the directory (/home/xxx/OpenFOAM/OpenFOAM-2.4.0/applications/utilities/mesh/conversion/ideasUnvToFoam) and run wmake after replacing it with the older ideasUnvToFoam.C version. If that the case for me what would be the newer version to use?and if it worked for me, is that enough to copy the polymesh generated case to my old case ( with old version )?
Many thanks in advance!
My best regards!


[Moderator note: Moved from IdeasUnvToFoam Bug amp Fix ]
Attached Images
File Type: jpg error_screen.jpg (86.7 KB, 76 views)
ugata88 likes this.

Last edited by wyldckat; August 27, 2017 at 10:28. Reason: see "Moderator note:"
alinuman15 is offline   Reply With Quote

Old   August 27, 2017, 10:32
Default
  #3
Retired Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,975
Blog Entries: 45
Rep Power: 128
wyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to all
Quick answer: As the message states:
Code:
Cell type 22 not supported
There was a bug report sometime ago about this... namely this one: https://bugs.openfoam.org/view.php?id=2627

Quoting from the answer I wrote there:
Quote:
That cell type 22 is not supported in any OpenFOAM version nor any fork or variant of OpenFOAM. Therefore, I doubt that this is even available on foam-extend 4, from where you got that "ideasUnvToFoam.C" file from.

Furthermore, cell type 22 is apparently a 2D cell, as indicated here: https://www.cfd-online.com/Forums/op...tml#post305957

Which means that the problem is that you are generating the mesh on Salome as a 2D mesh. You need to extrude the mesh into 3D and then export it to UNV, in order for it to be importable into OpenFOAM.

I'm closing this report, since there isn't much to be done here and it's borderline user support. And as a possible future feature, supporting 2D import from UNV format seems to me as a redundant effort, since Salome should be able to extrude the 2D mesh into 3D with the least amount of effort.
lourencosm and alinuman15 like this.
__________________
wyldckat is offline   Reply With Quote

Old   August 28, 2017, 15:48
Default
  #4
Member
 
Ali Noaman Ibrahim
Join Date: Sep 2015
Location: US_Chicago
Posts: 97
Rep Power: 10
alinuman15 is on a distinguished road
Thank you for replying. That bug report was reported by me under my university email
alinuman15 is offline   Reply With Quote

Old   August 30, 2017, 18:02
Default
  #5
Member
 
Hooman
Join Date: Apr 2011
Posts: 35
Rep Power: 15
hooman.4028 is on a distinguished road
I have the same problem.

cell type 22 not supported.

It is a 3D mesh from salome. What is the solution for this?

I simply made a face and extruded in 3D. The mesh looks perfectly fine with 1 layer of mesh in the 3D dimension, exactly what I am looking for.
hooman.4028 is offline   Reply With Quote

Old   August 30, 2017, 18:30
Smile
  #6
Member
 
Ali Noaman Ibrahim
Join Date: Sep 2015
Location: US_Chicago
Posts: 97
Rep Power: 10
alinuman15 is on a distinguished road
Quote:
Originally Posted by hooman.4028 View Post
I have the same problem.

cell type 22 not supported.

It is a 3D mesh from salome. What is the solution for this?

I simply made a face and extruded in 3D. The mesh looks perfectly fine with 1 layer of mesh in the 3D dimension, exactly what I am looking for.
Dear Hooman:-
As you might read the previous posts, mesh 22 is a 2D mesh, therefore, you have to extrude it with the appropriate mesh settings and then extrude it as .UNV. However, my advice to you, to mesh the surface effectively with fast simple way using Salome do the following:-
1. Create your 3D geometry (includes the target surface) and explode that geometry into faces.
2. Make automatic mesh setting choosing the suitable hypothesis for your geometry ( 3D-Hexahedralization, 3D-Tetrahedralization, ..etc).
3. Create mesh on geometry to including the target surface to have it meshed and reported as a patch for OpenFOAM.
Hope that makes sense for you.
my best.
hooman.4028 and Annier like this.
alinuman15 is offline   Reply With Quote

Old   August 30, 2017, 19:07
Default
  #7
Member
 
Hooman
Join Date: Apr 2011
Posts: 35
Rep Power: 15
hooman.4028 is on a distinguished road
Quote:
Originally Posted by alinuman15 View Post
Dear Hooman:-
As you might read the previous posts, mesh 22 is a 2D mesh, therefore, you have to extrude it with the appropriate mesh settings and then extrude it as .UNV. However, my advice to you, to mesh the surface effectively with fast simple way using Salome do the following:-
1. Create your 3D geometry (includes the target surface) and explode that geometry into faces.
2. Make automatic mesh setting choosing the suitable hypothesis for your geometry ( 3D-Hexahedralization, 3D-Tetrahedralization, ..etc).
3. Create mesh on geometry to including the target surface to have it meshed and reported as a patch for OpenFOAM.
Hope that makes sense for you.
my best.
Thank you very much, when
I assign empty to the 3d dimension patches, OpenFoam complaints that:

patch type 'patch' not constraint type 'empty'

I guess OpenFoam is still taking this as a 3D mesh and thus empty cannot be used. What would be your suggestion?
hooman.4028 is offline   Reply With Quote

Old   August 30, 2017, 19:43
Default ideasUnvToFoam Cell type not supported
  #8
Member
 
Ali Noaman Ibrahim
Join Date: Sep 2015
Location: US_Chicago
Posts: 97
Rep Power: 10
alinuman15 is on a distinguished road
When you set the patch to the option empty, that means :- the whole 3rd dimension is one cell unit. Therefore you can not discretize it into many cells.
Have a look at the following:-
http://www.salome-platform.org/forum/forum_10/904512484


Sent from my iPhone using CFD Online Forum mobile app
wyldckat, hooman.4028 and Annier like this.
alinuman15 is offline   Reply With Quote

Old   January 3, 2018, 06:02
Default
  #9
Member
 
Anil Kunwar
Join Date: Jun 2013
Posts: 64
Rep Power: 11
Annier is an unknown quantity at this point
Hi All,
I also encountered through this "Cell Type 22 Not Supported" situation and Thank you for your valuable discussions (as these experiences of you all have helped me a lot).
I made a cube geometry in Salome 7.8.0 software.
The Unv to polyMesh conversion was smooth or succesful for the following Mesh Applied Algorithms:
1. Netgen 3D, Mefisto 2D and Regular 1D.
2. Netgen_2D3D (I clicked Netgen 1D-2D-3D.) - the attachment below consists results for p at t=5 for hotRoom(buoyantBoussinesqPimpleFoam) tutorial performed with this mesh.


Yours Sincerely,
Anil Kunwar
Attached Images
File Type: png p5.png (152.5 KB, 34 views)
Annier is offline   Reply With Quote

Old   January 3, 2018, 06:54
Default
  #10
Member
 
Ali Noaman Ibrahim
Join Date: Sep 2015
Location: US_Chicago
Posts: 97
Rep Power: 10
alinuman15 is on a distinguished road
Quote:
Originally Posted by Annier View Post
Hi All,
I also encountered through this "Cell Type 22 Not Supported" situation and Thank you for your valuable discussions (as these experiences of you all have helped me a lot).
I made a cube geometry in Salome 7.8.0 software.
The Unv to polyMesh conversion was smooth or succesful for the following Mesh Applied Algorithms:
1. Netgen 3D, Mefisto 2D and Regular 1D.
2. Netgen_2D3D (I clicked Netgen 1D-2D-3D.) - the attachment below consists results for p at t=5 for hotRoom(buoyantBoussinesqPimpleFoam) tutorial performed with this mesh.


Yours Sincerely,
Anil Kunwar


Hi Anil:-
At that point, do you need any help?
My best.
alinuman15 is offline   Reply With Quote

Old   January 3, 2018, 09:00
Default
  #11
Member
 
Anil Kunwar
Join Date: Jun 2013
Posts: 64
Rep Power: 11
Annier is an unknown quantity at this point
Quote:
Originally Posted by alinuman15 View Post
Hi Anil:-
At that point, do you need any help?
My best.
Hi Ali,
I have found that you have put a lot of efforts on mesh export related works in Salome and OpenFoam. I appreciate your endeavours.
With Netgen_2D3D, the simulation run is successful.
Do you have any ideas on how we can assure 3D mesh (format) for the following Applied Algorithms in salome software:
1. Body Fitting Applied Algorithm
2. Netgen 2D, Netgen 3D (They are clicked separately in options for algorithm; Moreover I ticked the options for second order and quadrangle mapping in context of Netgen 2D applied algorithm)?
Also, I am interested in hexahedral mesh in Salome. Do you use them for your OpenFOAM simulations (If so what are the applied algorithms and hypotheses in Salome)?

Yours Sincerely,
Anil Kunwar
Annier is offline   Reply With Quote

Old   January 3, 2018, 09:25
Default
  #12
Member
 
Ali Noaman Ibrahim
Join Date: Sep 2015
Location: US_Chicago
Posts: 97
Rep Power: 10
alinuman15 is on a distinguished road
Quote:
Originally Posted by Annier View Post
Hi Ali,
I have found that you have put a lot of efforts on mesh export related works in Salome and OpenFoam. I appreciate your endeavours.
With Netgen_2D3D, the simulation run is successful.
Do you have any ideas on how we can assure 3D mesh (format) for the following Applied Algorithms in salome software:
1. Body Fitting Applied Algorithm
2. Netgen 2D, Netgen 3D (They are clicked separately in options for algorithm; Moreover I ticked the options for second order and quadrangle mapping in context of Netgen 2D applied algorithm)?
Also, I am interested in hexahedral mesh in Salome. Do you use them for your OpenFOAM simulations (If so what are the applied algorithms and hypotheses in Salome)?

Yours Sincerely,
Anil Kunwar
Hi Anil:-
1. for Body fitting application, look at the following video:-
https://www.youtube.com/watch?v=4xmSjjoioxI

2. Yes, they are separated ( but I did not get your point about them). For hexahedral mesh, I would say first start automatic hexahedralization ; if it does not succeed, split your geometry into blocks such that you could hexahedralize each separately under the whole geometry umbrella ( use submesh for each !).
My best
alinuman15 is offline   Reply With Quote

Old   January 14, 2018, 05:56
Default
  #13
Member
 
Anil Kunwar
Join Date: Jun 2013
Posts: 64
Rep Power: 11
Annier is an unknown quantity at this point
Hi Ali,
Thank you for your prompt and detailed response. The reference video for bodyfitting mesh application is very helpful.
1. About Netgen : I just meant that they are clicked separately as there are two options in Salome 7.8.0
as: (i) Netgen_2D3D (ticking it once will do both 2D and 3D
(ii) (a) Netgen-2D (tick it once separately)
(b) Netgen-3D (tick it again separately)

With option (i) , I could manage to have simulation successful and so I am asking you whether the second option has some difference with the first or not.

2. About Hexahedrons: The idea of sub-meshes with hexahedral multibodies seems to be a wonderful one. I will give it a try.

Yours Sincerely,
Anil Kunwar
Annier is offline   Reply With Quote

Old   January 20, 2018, 15:55
Default
  #14
Member
 
Anil Kunwar
Join Date: Jun 2013
Posts: 64
Rep Power: 11
Annier is an unknown quantity at this point
An additional note on ideasUnvToFoam
Code:
--> FOAM FATAL IO ERROR: 
cannot find file

file: /home/username/OpenFOAM_projects/tests/buoyantBoussinesqPimpleFoam/jouleHeating/system/controlDict at line 0.

    From function regIOobject::readStream()
    in file db/regIOobject/regIOobjectRead.C at line 72.

FOAM exiting
This can occur if controlDict is not available during Mesh conversion.

The availability of controlDict file inside system folder of the test directory is the necessary condition for successful mesh conversion from Unv to Foam format.

Yours Sincerely,
Anil Kunwar
Annier is offline   Reply With Quote

Old   January 20, 2018, 18:04
Default
  #15
Member
 
Ali Noaman Ibrahim
Join Date: Sep 2015
Location: US_Chicago
Posts: 97
Rep Power: 10
alinuman15 is on a distinguished road
Thanks Anil!
As far as I see from the error message:- this is something relating to the solver and no thing to do with the UnvToFoam.
Regards
alinuman15 is offline   Reply With Quote

Old   January 21, 2018, 03:03
Default
  #16
Member
 
Anil Kunwar
Join Date: Jun 2013
Posts: 64
Rep Power: 11
Annier is an unknown quantity at this point
Ali,
- I agree that it is related to Solver and ideasUnvToFoam.C is also one of the OpenFoam code. However, if we convert Unv geometry to Foam format within the test files containing all the minimum OpenFoam prerequisite files (i.e. including controlDict), there is no any issue of mesh conversion.
-I had tried one by one for all the files within the system directory and only upon the presence of controlDict file, the conversion of mesh from Unv to Foam proceeeds for buoyantBoussinesqPimpleFoam application. I hope this is generic to every OpenFoam application.


Yours Sincerely,
Anil Kunwar
Annier is offline   Reply With Quote

Old   December 11, 2020, 13:39
Default
  #17
New Member
 
M Shaaban
Join Date: Jun 2019
Posts: 9
Rep Power: 6
wildemam is on a distinguished road
I've faced this issue, and think it is related to the "second order' option in NetGen 1D-2D-3D parameters.
Sachin m and Desimuser1 like this.
wildemam is offline   Reply With Quote

Old   July 11, 2021, 19:39
Default
  #18
New Member
 
Juan Vera
Join Date: Jul 2021
Posts: 1
Rep Power: 0
jveraz is on a distinguished road
It worked for me not put any hypotheses in 2D-1D mesh option (I used hexahedrom algorithm).
jveraz is offline   Reply With Quote

Old   June 3, 2022, 05:59
Default
  #19
Member
 
Sachin
Join Date: Aug 2014
Location: India
Posts: 84
Rep Power: 11
Sachin m is on a distinguished road
The solution to this issue is to uncheck the option "second order" inside netgen parameters.
Desimuser1 likes this.
Sachin m is offline   Reply With Quote

Old   September 15, 2022, 22:46
Default Thanks!
  #20
New Member
 
Yeongbae Jeon
Join Date: Sep 2022
Posts: 1
Rep Power: 0
Yeongbae is on a distinguished road
Quote:
Originally Posted by Sachin m View Post
The solution to this issue is to uncheck the option "second order" inside netgen parameters.
God, you just saved my day
Yeongbae is offline   Reply With Quote

Reply

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
second order schemes marine OpenFOAM 67 April 11, 2022 18:19
High nut values in random place and time krzychu111 OpenFOAM Running, Solving & CFD 0 January 9, 2019 08:42
Compression instead of expansion EnricoDeFilippi OpenFOAM Running, Solving & CFD 1 October 8, 2018 10:19
Strange high velocity in centrifugal pump simulation huangxianbei OpenFOAM Running, Solving & CFD 26 August 15, 2014 02:27
SimpleFoam - instable simulation Specialist OpenFOAM Running, Solving & CFD 17 August 12, 2014 04:52


All times are GMT -4. The time now is 20:40.