[lam]

Oooh, sorry, for this silly question (how to use checkMesh)!!

But I think that I can have trouble if I don't know how to use "-autoInvert", don't I?

Lam

[rafal]

checkMesh <root> <case>

ie. for cavity in icoFoam

$ run
$ cd tutorials/icoFoam
$ checkMesh . cavity

[lam]

Thanks Rafal,

I have already managed to use "checkMesh", no problem.
But it's "-autoconvert" that I do not know to use.
CAn you help me?

Thanks in advance.
Lam

[rafal]

discuss ate last line of my previous post:
gmshToFoam <root> <case> <.msh> -autoInvert
i would try this and read all messages. there is also -verbose flag which gives you more info

[rafal]

discuss ate last line of my previous post:
gmshToFoam <root> <case> <.msh> -autoInvert
i would try this. There is also -verbose flag which gives you more info

[lam]

Thamks a lot Rafal,

I will try this command when I will be face to a complex mesh.

Regards,

Lam

[kmurphy]

Hi,

I am using OpenFOAM on a 2D problem (with two regions) and am having convergence issues. I think this may be due to the (poor) mesh that I have generated with blockMesh and wish to try a mesh generated by GMSH. However when I try to transform a .msh file using gmsh2ToFoam I get the error

FOAM FATAL ERROR : faces deallocated

I have read (and I think understood) the other posts that have referred to this error. In those post the grids being generated were 3D while in this case I want to generate a 2D grid.

Is it possible to import a 2D grid from GMSH?
Or if anyone has an 2D example or can tell what step I may have missed I would appreciate it.

Thanks in advance,
Kieran

[7islands]

Hi kmurphy,
As you know all the OpenFOAM meshes (and the meshes its converters handle) need to be 3D. To solve a 2D case you need to construct a 3D mesh with one cell height in Gmsh.

How about using the Extrude command? For example the following is extruding a 2D mesh of a square (meshed by triangles) to a 3D mesh (with prisms):

Point(1)={0,0,0,.1};Point(2)={1,0,0,.1};Point(3)={ 1,1,0,.1};Point(4)={0,1,0,.1};
Line(5)={1,2};Line(6)={2,3};Line(7)={3,4};Line(8)= {4,1};
Line Loop(9)={5,6,7,8};Plane Surface(10)={9};
Extrude {0,0,1}{Surface{10};Layers{1};Recombine;}

Takuya

[kmurphy]

Hi Takuya,

Thanks, that is exactly the effect that I was trying to get. In my attempts of a 3D representations of my 2D problem I had screwed up by ignoring the Layers command.

Regards,
Kieran

[marziolettich]

Hi everybody!
I tried to import a .msh file using gmshToFoam. Everything seems to have gone the right way (it created the right files in the right place, the mesh is visible with paraFoam) BUT all the external faces have been put in one patch, so it's very difficult to give to OpenFOAM the right boundary conditions (it would be a nasty work to separate the patches manually). I'm using gmsh 2.0.8 with OpenFOAM 1.4.1 on a linux Fedora machine.
Hope someone can help, thanks!
Marzio

[francesco_b]

Hi Marzio,

You should define your boundary faces as Physical groups before the import of the file. Then you can edit the files to put the right boundary conditions.

Regards,

Francesco

[7islands]

And also don't forget to define your internal mesh as a physical volume.

T.

[jason]

Hi,

I usually use the utility autoPatch or the other utility patchTool which I think you can find on the wiki. The patchTool utility lets you play around with the patches (select/name/merge/delete etc) in its own graphics window. I find it very useful for setting up boundary conditions.

Regards

Jason

[marziolettich]

Thanks! I would have never expected to get an answer so quickly! I've just started with gmesh and I will try to use your suggestion soom. In the meanwhile, I've found a compromise: if you use an older version than gmesh (I've just tried 1.65.0), the gmshToFoam utility creates a patch for each of the surfaces that define the original volume. Well, this could be annoying if most of them are of the same physical type (and would need to be grouped together), but it doesn't compromise the import.
Grazie ancora e ciao!
Marzio

[rafal]

try also gmsh2ToFoam found somewhere on Wiki or forum

[marziolettich]

Well, this must be the most efficient MessageBoard in the whole CFD community!
Thank you everybody.. I suppose that the surfaces you don't explicitly put in a physical group are treated as a unique "default group", or am I wrong?
Anyway, I will try each suggestion.
Thank you again (I wrote this in italian language in my previous message because I've read only Francesco's reply)
Marzio

[7islands]

Hi Marzio,
gmsh2ToFoam uses the elementary surface definitions when no physical group definition is found (which is the behavior much like gmshToFoam + Gmsh-1.65.0). If that's sufficient for you I also recommend gmsh2ToFoam [1].

[1] http://openfoamwiki.net/index.php/Contrib_gmshFoam

Takuya

[marziolettich]

Thank you Takuya! The whole project gmshFoam is quite interesting.
Once I have compiled with wmake the gmsh2ToFoam source OpenFOAM should recognize the command as any other utility or there's some other thing I should do?
Bye,
Marzio

[7islands]

To build gmsh2ToFoam unpacking the .tar.gz and running ./Allwmake is all you have to do.

T.

[marziolettich]

I know I'm abusing your patience... I must treat gmsh2ToFoam as a user-written application, right? So I untarred it and then I used wmake (I follow the OF manual). In this way, I need to specify the path every time I want to use gmsh2ToFoam or there's a variable I must set to make the command recognizable in every folder in the OF tree? I also run ./Allwmake as you said, to be true it's still running! I need to understand these matters since I'll have to modify some solvers and utilities to go on with my project and it would be very impractical if I had to recompile everything each time. I know I sound a little naive and I recognize there are many newbies like me that keep making the same questions but the search tool doesn't work and I'm not able to find a straight answer to my doubts.
Thank you and regards,
Marzio