[alinuman15]

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:-

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

[alinuman15]

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 From your old suggestion about similar case I knew that the solution is to find a newer version of the file ideasUnvToFoam.C in the directory (/home/xxx/OpenFOAM/OpenFOAM-2.4.0/applications/utilities/mesh/conversion/ideasUnvToFoam) and run wmake after replacing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 ]

[wyldckat]

Quick answer: As the message states:

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:

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.

[alinuman15]

Thank you for replying. That bug report was reported by me under my university email

[hooman.4028]

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.

[alinuman15]

Originally Posted by hooman.4028

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]

Originally Posted by alinuman15

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?

[alinuman15]

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

[Annier]

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

[alinuman15]

Originally Posted by Annier

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.

[Annier]

Originally Posted by alinuman15

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

[alinuman15]

Originally Posted by Annier

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

[Annier]

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]

An additional note on ideasUnvToFoam

--> 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

[alinuman15]

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

[Annier]

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

[wildemam]

I've faced this issue, and think it is related to the "second order' option in NetGen 1D-2D-3D parameters.

[jveraz]

It worked for me not put any hypotheses in 2D-1D mesh option (I used hexahedrom algorithm).

[Sachin m]

The solution to this issue is to uncheck the option "second order" inside netgen parameters.

[Yeongbae]

Originally Posted by Sachin m

The solution to this issue is to uncheck the option "second order" inside netgen parameters.

God, you just saved my day