[Ingöö]

Hi,

I'm trying to create a mesh around a NACA 0015 airfoil using foam-extend-3.1 with snappyHexMesh. I have already run the surfaceFeatureExtract command to create an eMesh file for the airfoil. I'm getting the following error message when I run the snappyHexMesh command:

Reading external feature lines

--> FOAM FATAL IO ERROR:
Expected a '(' while reading VectorSpace<Form, Cmpt, nCmpt>, found on line 19 the word 'externalStart'

file: /Volumes/foam-extend-3.1/tutorials/multiphase/interFoam/ras/NACA0015Test/constant/triSurface/NACA0015.eMesh at line 19.

    From function Istream::readBegin(const char*)
    in file db/IOstreams/IOstreams/Istream.C at line 86.

FOAM exiting

I have uploaded my test case to dropbox.
https://www.dropbox.com/s/45nv9u8le7...015%20Test.zip

snappyHexMesh runs without any errors when I comment out the featureEdgeMesh in snappyHexMeshDict. But it seems to ignore my stl file because I cannot see the NACA airfoil in the mesh.

I really appreciate any help you can provide.

Ingöö

[student666]

Expected a '(' while reading VectorSpace<Form

seems OpenFoam already told you the problem.

Have a look at your emesh file go to line 19 and check for the missing (, maybe you edited it with no intentions.

[Seroga]

Is it possible to use snappyHexMesh without emesh-files?

[stephie]

Hello everyone,

I am trying to use SnappyHexMesh to snap a foil geometry out of an rectangular (small box).
I use the foam extend 3.1 version. Unfortunately I am not able to produce an emesh. Could anyone help me or send me the correct command? I would be very grateful.

These are the commands I used:

ideasUnvToFoam cad/name.unv

surfaceFeatureExtract -includedAngle 150 constant/triSurface/name.stl name

(here the eMesh normaly is produced..but the command just produce the .obj files)

snappyHexMesh -overwirte

--> here I gut this message because of the missing emesh file

--> FOAM FATAL IO ERROR:
problem while reading header for object foil_mesh.eMesh

file: /home/stephanie/Schreibtisch/SnappyHexMesh_NACA4518_150611/adaptiveMesh/constant/triSurface/foil_mesh.eMesh at line 2.

From function regIOobject::readStream()
in file db/regIOobject/regIOobjectRead.C at line 69.

FOAM exiting


best regards,
Stephie

[student666]

You can use surface feature exctract with stl files. Ideas unv to foam, already convert the unv file into openfoam mesh.

[stephie]

Yes that is correct and what I do.

My background box is an .unv file which I convert to OpenFoam first.

The geometry of the foil is a stl file, which I would like to snap out of the box.

How I wrote, I use the following command surfaceFeatureExtract -includedAngle 150 constant/triSurface name.stl name

My current problem is, that this command does not produce any eMesh file.

So I guess, the command is not correct?

[student666]

Ok, now I get it, I think the command is right.

Maybe a trivial error, you have to set the name of the stl file, not the name of your background mesh

surfaceFeatureExtract -includedAngle 150 constant/triSurface/name.stl name

I would change to

surfaceFeatureExtract -includedAngle 150 constant/triSurface/foil.stl

or whatever the name of your file is.

In any case I generally use a surfaceFeatureExctractDict in the system directory like:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.3.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      surfaceFeatureExtractDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

amiRot1.stl
{
    extractionMethod    extractFromSurface; // extractFromFile or extractFromSurface
    extractFromSurfaceCoeffs
    {includedAngle   135;}
    writeObj                yes;    // Write options
}

then I only type surfaceFeatureExctract in the main root of the case.

[stephie]

Hey,

thank you for your support. But the stl name is okay and here is my surfaceFeatureExtractDict

/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.3.1 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object surfaceFeatureExtractDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

foil_mesh.stl
{
// How to obtain raw features (extractFromFile || extractFromSurface)
extractionMethod extractFromSurface;

extractFromSurfaceCoeffs
{
// Mark edges whose adjacent surface normals are at an angle less
// than includedAngle as features
// - 0 : selects no edges
// - 180: selects all edges
includedAngle 150;
}

// Write options

// Write features to obj format for postprocessing
writeObj yes;
}


// ************************************************** *********************** //

May I send you a dropbox link with my case?

[student666]

ok. I'll wait for it. I'll give it a try. You can post it here, or send to e-keneso@libero.it

[wyldckat]

Quick answer:

1. I'm not certain if snappyHexMesh in foam-extend 3.1 is able to handle feature edges, because I can't find any tutorial for them.
2. You could have taken a look at the tutorial cases in OpenFOAM 2.0 and newer did it:
   

   surfaceFeatureExtract -includedAngle 150 constant/triSurface/name.stl constant/triSurface/name.eMesh

(edit: Moved my post for the answer I gave for the repeated question that was made on another thread.)

[student666]

Hi,

i performed some tests, but verify yourself what I'm writing:

Foam extended 3.1 can't perform the command surfaceFestureExctract with a dictionary in the system folder, f I type the command surface feature extract in Foam ext. I got this error message:

Usage:  surfaceFeatureExtract <surface> <output set> [-minElem  number of edges in feature] [-minLen cumulative length of feature]  [-deleteBox ((x0 y0 z0)(x1 y1 z1))] [-subsetBox ((x0 y0 z0)(x1 y1 z1))]  [-set input feature set] [-includedAngle included angle [0..180]] [-case  dir] [-noFunctionObjects]  [-help] [-doc] [-srcDoc]

So in order to extract the edges i used openfoam 2.4.0 or 2.3.1; with these versions I have been able to extract the edges. Somewhere on the web, I red about some problem with snappyHexMesh and foam extended version, but I didn't save the link, so you have to look for information if this is true. My suggestion is then to perform meshing operation with standard OF.

I wasn't able to open neither the stl file and the edges file with paraview, It crashes all the time, only blender gave me support; I suggest you to export the stl in other ways, cause it seems that your cad program is not performing it so good.

Hope this can help.

Ciao

Michele

[stephie]

Hallo Michele, hello Bruno,

thank you for your support.
Finally I used your hint and create the emesh with OpenFOAM 2.4 and put it into foam-extend.
Now it works...today I was able to snap the foil geometry into the backgroundmesh.

best regards,
Stephie

[Rakkiran]

Hello Foamers,
I know this is very old post but I am facing few issues with eMesh. When I run the command surfaceFeatureExtract it is giving .eMesh files with zero points and zero edges .
Couldn't figure out the reason.


Regards,
Raj Kiran.

[wyldckat]

Originally Posted by Rakkiran

When I run the command surfaceFeatureExtract it is giving .eMesh files with zero points and zero edges .

Quick answer:

surfaceCheck constant/triSurface/yourFileName.stl

this will give you information on the status and summary details of the STL file.