[AleDR]

Hi FOAMers!

I have some problems with mesh file conversion!!
I'm trying to import NASA grid for the flat plate test case in OpenFOAM... but I don't know how to!!
I am puzzled by the file extension... .p3dmft ? It should be a PLOT3D file format, but I couldn't handle it in ParaView.

I tried the plot3dToFoam but I got this error:

Create time

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

file: flatplate_clust2_4levelsdown_35x25.p3dmft at line 1.

From function void Istream::getBack(token&)
in file db/IOstreams/IOstreams/Istream.C at line 38.

FOAM exiting

Can anybody help me? Thanks!

[kiddmax]

Hey Alessandro

Did you solve the problem?

Best
Ye

[VincentHUBER]

I'm highly interested in the issue ! Have you successfully converted the mesh ?

[alexeym]

Hi,

I was not successful in converting meshes with OpenFOAM's plot3dToFoam (and any way there is not much sense in converting just geometry), so I have created Python script for conversion from Plot3D to Gmsh (https://github.com/mrklein/p3d2gmsh) then you can use gmshToFoam to convert mesh into OpenFOAM's format.

In general you will need geometry file (*.p3dfmt) and Neutral Map File with description of boundary conditions. I have tested the script on verification cases from http://turbmodels.larc.nasa.gov, it seems to be converting the meshes and BCs correctly.

[VincentHUBER]

Wonderfull ! (Actually, I was planning to get Gmsh mesh files :-) )

Bonus questioon
- do you know a way to get the 3D gmsh mesh in 2D (cut along a plane) ?
OR
- can your script (that I ran successfully) be applied to p2dfmt ... without the neutral map file ?

[alexeym]

No, I don't know the way to flatten mesh in Gmsh. In OpenFOAM there us flattenMesh utility, though its output is a point field, i.e. there will be no information about edges, boundaries, etc. Also there is Gmsh plugins like CutPlane, but again it will lose boundary information.

Initially I started with p2dfmt files but then realized there is no information on boundary conditions, so I've abandoned the idea.

[makayasa]

hi alexym, after seraching how to convet plot3dtoFoam finally I find this forum. But i get error message when running sript p3d2gmsh.py. How do fix this?


Can't open [-o. Skipping.
Can't open naca0012]. Skipping.
Can't open [-m. Skipping.
Can't open n0012]. Skipping.

[alexeym]

Hi,

Your output suggests that you have decided to copy command line with brackets (i.e. [-o naca0012] instead of just -o naca0012), while command should be something like:

./p3d2gmsh.py -o naca0012.msh -m naca0012.nmf naca0012.p3d

This is just a guess and could be irrelevant, since your post lacks information on the way you have got the error.

[makayasa]

Thanks for reply alexym.
After run command ./p3d2gmsh.py -o naca0012.msh -m naca0012.nmf naca0012.p3d
I am get error message :

Traceback (most recent call last):
File "./p3d2gmsh.py", line 585, in <module>
main()
File "./p3d2gmsh.py", line 577, in main
nmf = NeutralMapFile(mapfile)
File "./p3d2gmsh.py", line 90, in __init__
fp = open(filename, 'r')
TypeError: coercing to Unicode: need string or buffer, list found

even tried the files in the folder test, but I still get the same error message. How to fix this?
Thank you

[alexeym]

Hi,

There was a bug (guess I have never really tested -o and -m flags). I have pushed fix to repository, so you need to re-download p3d2gmsh.py script.

[makayasa]

Its work
So, I went on the next stage of the run command gmshToFoam but I get the following message

#0 Foam::error:rintStack(Foam::Ostream&) in "/home/xxx/OpenFOAM/OpenFOAM-1.7.1/lib/linuxGccDPOpt/libOpenFOAM.so"
#1 Foam::sigSegv::sigSegvHandler(int) in "/home/xxx/OpenFOAM/OpenFOAM-1.7.1/lib/linuxGccDPOpt/libOpenFOAM.so"
#2 Uninterpreted:
#3
in "/home/xxx/OpenFOAM/OpenFOAM-1.7.1/applications/bin/linuxGccDPOpt/gmshToFoam"
#4 __libc_start_main in "/lib/i386-linux-gnu/libc.so.6"
#5
in "/home/xxx/OpenFOAM/OpenFOAM-1.7.1/applications/bin/linuxGccDPOpt/gmshToFoam"
Segmentation fault (core dumped)

Thank you

[alexeym]

This time I can not guess what went wrong, since I have never used version 1.7.1 (well, except certain portions of foam-extent 3.1, which turned your to be OpenFOAM 1.7.x) and you did not show the way to reproduce your error.

[makayasa]

The way that I use :
1.from (http://turbmodels.larc.nasa.gov/naca0012_grids.html) i get file to convert msh file
2. I used a python script from ( https://github.com/mrklein/p3d2gmsh ) to convert msh file
3. I moved the msh file to folder $ FOAM_RUN
4. then use the command gmshToFoam . And I got a message as I have mentioned
whether there are less of these steps ? please correction

[alexeym]

I can not reproduce the error neither with OpenFOAM 2.4.x, nor with 3.0.x. So I guess, it is specific to 1.7.1 and I do not know how to fix it.

[makayasa]

Thank you so much for your help. Maybe I 'll try openfoam 2.4.0

[Flowkersma]

Hi,

Just for record. I have successfully converted the meshes from NASA page with plot3dToFoam converter by adding -noBlank parameter. For example:

2D mesh

plot3dToFoam naca0012.p2dfmt -2D 1 -noBlank

3D mesh

plot3dToFoam naca0012.p3dfmt -noBlank

I had also problems on converting the p3d meshes created by Construct2D.
I solved it by adding a line with 1 in the beginning of the p3d file. For boundary conditions, I use autoPatch and createPatch utilities.

Regards,
Mikko

[aero_cfd]

Originally Posted by alexeym

Hi,

I was not successful in converting meshes with OpenFOAM's plot3dToFoam (and any way there is not much sense in converting just geometry), so I have created Python script for conversion from Plot3D to Gmsh (https://github.com/mrklein/p3d2gmsh) then you can use gmshToFoam to convert mesh into OpenFOAM's format.

In general you will need geometry file (*.p3dfmt) and Neutral Map File with description of boundary conditions. I have tested the script on verification cases from http://turbmodels.larc.nasa.gov, it seems to be converting the meshes and BCs correctly.

HI,
Thanks for this script , I am trying to use the PLOT3D meshes in ansys and therefore I want to convert them, I execute the script but it takes sometime and still nothing, does it usually take long to convert ?

Thanks

[TheOneBird]

Thank you heaps for your script. It works great. Firstly, apologies for commenting on such an old thread however I thought this was the best place to post this.

I am having issues setting up one of the NASA cases. 9https://turbmodels.larc.nasa.gov/jetsubsonic_grids.html). The problem I am facing is that the internal faces, between the blocks, appear as boundary conditions in the FOAM file format. It appears that when I run the case, it does not recognise them as internal faces and the solution has discontinuities at each interface. I have set the face type in "boundaries" to "empty", however this has not helped.

Is it possible for someone to share a case directory where they have successfully run one of the NACA cases please? Or could someone direct me in the correct direction for fixing this. Thanks!

[mlsk]

Hi guy, i want in import the Plot3Dmesh file(raetaf.x.fmt) to openFoam.
I have tried all the commands i amaware of from the documentation and this Forum.I am facing this issue:

FOAM FATAL IO ERROR:
wrong token type - expected int32_t, found on line 2 the doubleScalar 27.00003

file: raetaf.x.fmt at line 2.

From function Foam::Istream& Foam:perator>>(Foam::Istream&, int32_t&)
in file primitives/ints/int32/int32IO.C at line 62.

It would veryhelpful if anyone can give me way out of this.

Thanks in advance.