[Gmsh] gmsh or gmshToFoam problem?
Louis Gagnon
louis.gagnon.10 at ulaval.ca
Wed Oct 30 01:55:31 CET 2013
For those still having a similar problem with the gmshToFoam utility, for me it turned out that the issue was due to a reduction of the write precision from 16 (gmsh) to 6 (OpenFoam). I was able to correct this by setting the appropriate precision in the system/controlDict:writePrecision entry of the OF case prior to running gmshToFoam. More details are given in Martin Beaudoin's post at http://www.cfd-online.com/Forums/openfoam-solving/88156-ggi-tolerance.html#post315867
Cheers,
-Louis
Le 19 juin 2012 à 14:46, Madeleine Vincent a écrit :
>
> gmsh friends -
>
> I have a question regarding gmsh and the gmshToFoam utility within OpenFOAM, one of which seems to be not acting as I had presumed.
>
> I have a simple mesh problem which I've distilled down to the it's basic form.
> I am running a gmsh script (.geo) to create a 3D rectangular flow field with a circular cylinder in the middle.
> When I run gmsh, it meshes succesfully. However, when I run gmshToFoam (conversion to the OpenFOAM polyMesh format), I end up with a mesh that is not usable.
>
Have you done gmsh -optimize, the optimizer is not put on by default : this will change in the next versions
JF
> First of all, I get a warning saying:
>
>
> [warning]
> --> FOAM Warning :
> From function polyMesh::polyMesh(... construct from shapes...)
> in file meshes/polyMesh/polyMeshFromShapeMesh.C at line 619
> Found 9022 undefined faces in mesh; adding to default patch.
> [/warning]
>
>
>
> Invoking the "checkMesh" utility results in the following errors:
>
>
> [error]
> Checking geometry...
> Overall domain bounding box (0 0 -0.75) (9 6 0.75)
> Mesh (non-empty, non-wedge) directions (1 1 1)
> Mesh (non-empty) directions (1 1 1)
> Boundary openness (1.15651e-17 5.07766e-19 9.032e-18) OK.
> ***High aspect ratio cells found, Max aspect ratio: 7.58943e+198, number of cells 3
> <<Writing 3 cells with high aspect ratio to set highAspectRatioCells
> Minumum face area = 6.81219e-06. Maximum face area = 0.177405. Face area magnitudes OK.
> Min volume = 1.33333e-300. Max volume = 0.0208743. Total volume = 80.8949. Cell volumes OK.
> Mesh non-orthogonality Max: 89.2144 average: 30.4407
> *Number of severely non-orthogonal faces: 1046.
> Non-orthogonality check OK.
> <<Writing 1046 non-orthogonal faces to set nonOrthoFaces
> ***Error in face pyramids: 8 faces are incorrectly oriented.
> <<Writing 8 faces with incorrect orientation to set wrongOrientedFaces
> Max skewness = 2.23263 OK.
> Coupled point location match (average 0) OK.
>
> Failed 2 mesh checks.
> [/error]
>
>
>
> The gmsh script (.geo file) is as follows:
>
>
> [script]
> // Everything is parameterized on the cylinder radius
> rad = 0.15;
>
> //Characteristic length - used for mesh sizing
> lc = 4*rad;
>
> //Plane dimesions
> planeLength = 60*rad;
> planeWidth = 40*rad;
>
> //Cyclinder constants
> cir_x = 15*rad; //The absolute X distance of the center
> cir_y = planeWidth / 2; //The absolute Y distance of the center
>
> //The bottom plane number
> bottomPlaneNum = 16;
>
> //The extrusion thickness
> extThickness = rad*10;
> zBottom = -(extThickness/2.0);
> zTop = (extThickness/2.0);
> z = zBottom; //The z-height of this plane.
> // NOTE - For 2D, the plane is centered at 0, so
> // the z value used will be -(h/2)
>
> //Rectangular plane (Counter-clockwise, starting in lower left corner)
> Point(1) = {0, 0, z, lc};
> Point(2) = {planeLength, 0, z, lc};
> Point(3) = {planeLength, planeWidth, z, lc};
> Point(4) = {0, planeWidth, z, lc};
>
> //Circle
> Point(5) = {cir_x, cir_y, z, lc}; // Center point
> Point(6) = {cir_x, cir_y + rad, z, lc}; // 12 o'clock
> Point(7) = {cir_x + rad, cir_y, z, lc}; // 3
> Point(8) = {cir_x, cir_y - rad, z, lc}; // 6
> Point(9) = {cir_x - rad, cir_y, z, lc}; // 9
>
> //Lines
> Line(1) = {1, 2};
> Line(2) = {2, 3};
> Line(3) = {3, 4};
> Line(4) = {4, 1};
> Circle(5) = {6, 5, 7};
> Circle(6) = {7, 5, 8};
> Circle(7) = {8, 5, 9};
> Circle(8) = {9, 5, 6};
> Line Loop(9) = {1, 2, 3, 4};
> Line Loop(10) = {5, 6, 7, 8};
>
> //Surface
> // Don't add any line loop(s) specific to meshing
> Plane Surface(bottomPlaneNum) = {9, 10};
>
> //Extrude the bottom surface in the z direction a total of extThickness units.
> // This extrusion is centered on 0 (from -h/2 to +h/2)
> newSurfs[] = Extrude {0,0,extThickness} {
> Surface{bottomPlaneNum};
> };
>
> //Name the surfaces
> Physical Surface("topAndBottom") = {bottomPlaneNum, newSurfs[0]};
> Physical Surface("nearAndFar") = {newSurfs[2], newSurfs[4]};
> Physical Surface("outlet") = {newSurfs[3]};
> Physical Surface("inlet") = {newSurfs[5]};
> Physical Surface("cylinder") = {newSurfs[9], newSurfs[8], newSurfs[7], newSurfs[6]};
>
> Physical Volume(1) = {newSurfs[1]};
>
> //Meshing
> fineness = 15;
>
> Field[4] = Cylinder;
> Field[4].Radius = 1.5*rad;
> Field[4].VIn = lc / fineness;
> Field[4].VOut = lc / 2;
> Field[4].XAxis = 0.0;
> Field[4].XCenter = cir_x;
> Field[4].YAxis = 0.0;
> Field[4].YCenter = cir_y;
> Field[4].ZAxis = 1.0;
> Field[4].ZCenter = 0.0;
>
> Field[6] = Box;
> Field[6].VIn = lc / (fineness / 3);
> Field[6].VOut = lc;
> Field[6].XMin = cir_x - 3*rad;
> Field[6].XMax = cir_x + 10*rad;
> Field[6].YMin = cir_y - 3*rad;
> Field[6].YMax = cir_y + 3*rad;
> Field[6].ZMin = zBottom -0.000001;
> Field[6].ZMax = zTop +0.000001;
>
> // Use minimum of all the fields as the background field
> Field[100] = Min;
> Field[100].FieldsList = {4, 6};
> Background Field = 100;
>
> [/script]
>
>
>
> I have no problem with the 2D case -- I use Layers{1} and Recombine within the extrusion command. This works well.
>
> I have also seen that using many layers within the 3D case will also produce a mesh that passes the checkMesh utility. But this doesn't provide a good 3D mesh, as the domain is segregated throughout in these distinct layers, and it doesn't take into account the finer meshing (in the Z direction) around the cylinder.
>
> So I'm wondering if this is an issue in the meshing of gmsh, or the gmshToFoam utility? And what remedy might be available.
>
> Thank you very much for any help you are able to provide.
>
> Madeleine P. Vincent
>
> _______________________________________________
> gmsh mailing list
> gmsh at geuz.org
> http://www.geuz.org/mailman/listinfo/gmsh
------------------------------------------------------------------
Prof. Jean-Francois Remacle
Universite catholique de Louvain (UCL)
Ecole Polytechnique de Louvain (EPL) - Louvain School of Engineering
Institute of Mechanics, Materials and Civil Engineering (iMMC)
Center for Systems Engineering and Applied Mechanics (CESAME)
Tel : +32-10-472352 -- Mobile : +32-473-909930
-------------- next part --------------
An HTML attachment was scrubbed...
URL: <http://www.geuz.org/pipermail/gmsh/attachments/20120622/192a499a/attachment.html>