CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Pre-Processing

LES 2D multiphase simulation error using imported gmsh mesh

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   April 13, 2015, 04:09
Default LES 2D multiphase simulation error using imported gmsh mesh
  #1
New Member
 
thomas
Join Date: Jul 2014
Posts: 8
Rep Power: 3
thomas. is on a distinguished road
Hello all,

I am trying to simulate a multiphase flow using interFoam and using LES for turbulence modelling. I will try to be as accurate as possible regarding the description of the problem, so I will quote all error/warnings messages from terminal.
I would really appreciate your help. Thanks in advance for your time!

So, the geometry file in gmsh is:

Code:
// Gmsh project created on Thu Apr  9 09:24:11 2015
el = 1;
pi = 3.14159265;
theta = (pi/4 + pi/2);
theta2 = (pi/4);
r = 40;
r2 = 40+20*Cos(theta2);

Point(1) = {0, 0, 0, el};
Point(2) = {0, 15, 0, el};
Point(3) = {r2*Cos(theta), 15+r2*Sin(theta), 0, el};
Point(4) = {r*Cos(theta), 35+r*Sin(theta), 0, el};
Point(5) = {0, 35, 0, el};
Point(6) = {0, 40, 0, el};
Point(7) = {120, 40, 0, el};
Point(8) = {120, 35, 0, el};
Point(9) = {160, 35, 0, el};
Point(10) = {160, 15, 0, el};
Point(11) = {120, 15, 0, el};
Point(12) = {120, 0, 0, el};
Line(1) = {1, 2};
Line(2) = {2, 3};
Line(3) = {3, 4};
Line(4) = {4, 5};
Line(5) = {5, 6};
Line(6) = {6, 7};
Line(7) = {7, 8};
Line(8) = {8, 9};
Line(9) = {9, 10};
Line(10) = {10, 11};
Line(11) = {11, 12};
Line(12) = {12, 1};
Line Loop(13) = {6, 7, 8, 9, 10, 11, 12, 1, 2, 3, 4, 5};
Plane Surface(14) = {13};

Extrude {0, 0, 10} {
  Surface{14};
  Layers{1};
  Recombine;
}
Physical Surface("back") = {14};
Physical Surface("front") = {76};
Physical Surface("inlet") = {67};
Physical Surface("outlet") = {43};
Physical Surface("walls") = {59, 63, 71, 75, 31, 35, 39, 43, 47, 55};
Physical Volume("interior") = {1};
After converting the mesh file using gmshToFoam, I get following warning:

Code:
--> FOAM Warning : 
    From function polyMesh:polyMesh(... construct from shapes...)
    in file meshes/polyMesh/polyMeshFromShapeMesh.C at line 627
    Found 248400 undefined faces in mesh; adding to default patch.
The resulting boundary file looks like this:

Code:
6
(
    back
    {
        type            patch;
        physicalType    patch;
        nFaces          122260;
        startFace       609360;
    }
    walls
    {
        type            patch;
        physicalType    patch;
        nFaces          3496;
        startFace       731620;
    }
    outlet
    {
        type            patch;
        physicalType    patch;
        nFaces          156;
        startFace       735116;
    }
    inlet
    {
        type            patch;
        physicalType    patch;
        nFaces          112;
        startFace       735272;
    }
    front
    {
        type            patch;
        physicalType    patch;
        nFaces          122260;
        startFace       735384;
    }
    defaultFaces
    {
        type            patch;
        nFaces          116;
        startFace       857644;
    }
)
As I change the type and physical type for front and back to "empty" while leaving the defaultFaces type as "patch" and I try to run interFoam, I get following error:

Code:
--> FOAM FATAL IO ERROR: 
Cannot find patchField entry for defaultFaces

file: /home/thomas/CFD/OpenFOAM/thomas-2.3.1/run/tutorials/multiphase/interFoam/thomasCaseLES/0/p_rgh.boundaryField from line 25 to line 42.

    From function GeometricField<Type, PatchField, GeoMesh>::GeometricBoundaryField::readField(const DimensionedField<Type, GeoMesh>&, const dictionary&)
    in file /home/opencfd/OpenFOAM/OpenFOAM-2.3.0/src/OpenFOAM/lnInclude/GeometricBoundaryField.C at line 209.

FOAM exiting
And if I change the defaultFaces type to "empty", I get following error:

Code:
--> FOAM FATAL ERROR: 
Case is not 3D or 2D, LES is not applicable

    From function cubeRootVolDelta::calcDelta()
    in file cubeRootVolDelta/cubeRootVolDelta.C at line 72.

FOAM exiting
Once again, thank you in advance for reading and trying to help!
thomas. is offline   Reply With Quote

Old   April 13, 2015, 04:27
Default
  #2
Senior Member
 
Alexey Matveichev
Join Date: Aug 2011
Location: Nancy, France
Posts: 1,114
Rep Power: 19
alexeym will become famous soon enoughalexeym will become famous soon enough
Hi,

You have forgotten to add one surface into walls patch (see attached image), so they went into defaultFaces and this ended with final error (as for 2D case only front and back should be empty).

Also, you have to edit boundary dictionary (with changeDictionary utility for example), so front and back have type empty, walls has type wall (or your next question will be about wall functions those complain about walls not being walls ).

And finally, why not make hexagonal mesh using transfinite algorithm? The geometry is very simple.
Attached Images
File Type: png default-faces.png (5.5 KB, 9 views)
alexeym is offline   Reply With Quote

Old   April 13, 2015, 07:56
Default
  #3
New Member
 
thomas
Join Date: Jul 2014
Posts: 8
Rep Power: 3
thomas. is on a distinguished road
Hi,

first of all, thank you very much for responding. Your comment helped me to find where I was messing up: I checked the wall boundaries definition and I noticed, that I had surface 43 defined as an outlet and as a wall. In stead of defining surface 43 as a wall, I have to define surface 51 as a wall.

Regarding the transfinite algoritm: that's the next step!

Thanks again!
thomas. is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Mesh motion with Translation & Rotation Doginal CFX 2 January 12, 2014 07:21
[ICEM] Getting the right mesh for simulation dcggames ANSYS Meshing & Geometry 9 January 8, 2013 10:51
No layers in a small gap bobburnquist OpenFOAM Native Meshers: snappyHexMesh and Others 2 November 25, 2012 09:54
Problem w/ vortex ring simulation, mesh coarseness parameters? ESC FLUENT 2 September 4, 2012 10:56
2D Mesh Generation Tutorial for GMSH aeroslacker Open Source Meshers: Gmsh, Netgen, CGNS, ... 12 January 19, 2012 04:52


All times are GMT -4. The time now is 01:14.