|
[Sponsors] |
![]() |
![]() |
#1 |
New Member
Join Date: Jan 2017
Posts: 5
Rep Power: 9 ![]() |
Hello everybody.
I am a beginner with Openfoam and I am trying to model the flow past a sphere with an axisymmetric study. I created my mesh with gmsh but when I am using gmshToFoam I have the following error message : Code:
Create time Starting to read mesh format at line 2 Read format version 2.2 ascii 0 Starting to read physical names at line 5 Physical names:8 Line 4 axis Surface 1 inlet Surface 2 outlet Surface 3 wall Surface 5 sphere Surface 6 front Surface 7 back Volume 8 interior Starting to read points at line 16 Vertices to be read:22920 Vertices read:22920 Starting to read cells at line 22939 Cells to be read:22685 Unhandled element 1 at line 22941 Unhandled element 1 at line 22942 ................ Unhandled element 1 at line 23035 Unhandled element 1 at line 23036 .............. Unhandled element 1 at line 23087 Mapping region 7 to Foam patch 0 Mapping region 8 to Foam cellZone 0 Cells: total:11269 hex :11137 prism:132 pyr :0 tet :0 CellZones: Zone Size 0 11269 Skipping tag at line 45627 Patch 0 gets name back --> FOAM Warning : From function Foam::polyMesh::polyMesh(const Foam::IOobject&, const Foam::Xfer<Foam::Field<Foam::Vector<double> > >&, const cellShapeList&, const faceListList&, const wordList&, const wordList&, const Foam::word&, const Foam::word&, const wordList&, bool) in file meshes/polyMesh/polyMeshFromShapeMesh.C at line 595 Found 22906 undefined faces in mesh; adding to default patch. Finding faces of patch 0 FaceZones: Zone Size Writing zone 0 to cellZone interior and cellSet End That is my .geo file so you will probably find the problem (I hope ![]() Code:
cl__1 = 1; Point(1) = {-100, 0, 0, 1}; Point(2) = {200, 0, 0, 1}; Point(3) = {-100, 100, 0, 1}; Point(4) = {200, 100, 0, 1}; Point(5) = {-7.5, 0, 0, 1.0}; Point(6) = {7.5, 0, 0, 1.0}; Point(7) = {0, 0, 0, 1.0}; Point(11) = {100, 0, 0, 1.0}; Point(12) = {100, 100, 0, 1.0}; //sphere Point(8) = {5.3033008589, 5.3033008589, 0, 1.0}; Point(9) = {-5.3033008589, 5.3033008589, 0, 1.0}; Point(10) = {5.3033008589, 5.3033008589, 0, 1.0}; //lignes domaine Line(1) = {3, 1}; Line(2) = {12, 11}; Line(3) = {4, 2}; Line(4) = {3, 12}; Line(5) = {12, 4}; Line(6) = {1, 5}; Line(7) = {6, 11}; Line(8) = {11, 2}; Line(95) = {5, 6}; //sphere Circle(9) = {5, 7, 9}; Circle(10) = {9, 7, 8}; Circle(11) = {8, 7, 6}; //lignes bloc Line(12) = {3, 9}; Line(13) = {12, 8}; Transfinite Line {4} = 60 Using Progression 1; Transfinite Line {5, 8} =15 Using Progression 1; Transfinite Line {1} = 60 Using Progression 1; Transfinite Line {2, 3} = 60 Using Progression 0.96; Transfinite Line {11, 10, 9} = 60 Using Progression 1; Transfinite Line {10} = 60 Using Progression 1; Transfinite Line {12} = 60 Using Progression 0.9; Transfinite Line {13} = 60 Using Progression 0.9; Transfinite Line {6} = 60 Using Progression 0.9; Transfinite Line {7} = 60 Using Progression 1.1; //surfaces Line Loop(14) = {12, 10, -13, -4}; Plane Surface(15) = {14}; Line Loop(16) = {12, -9, -6, -1}; Plane Surface(17) = {16}; Line Loop(18) = {13, 11, 7, -2}; Plane Surface(19) = {18}; Line Loop(20) = {5, 3, -8, -2}; Plane Surface(21) = {20}; Transfinite Surface {17}; Transfinite Surface {15}; Transfinite Surface {19}; Transfinite Surface {21}; Recombine Surface {17}; Recombine Surface {15}; Recombine Surface {19}; Recombine Surface {21}; Extrude {{1,0,0}, {0,0,0},Pi/36} { Surface{17, 15, 19, 21}; Layers{1}; Recombine; } Physical Surface("inlet") = {37};//inlet Physical Surface("outlet") = {89};//outlet Physical Surface("wall") = {59, 86};//wall haut Physical Line("axis") = {6, 7, 8, 95};//ligne sym Physical Surface("sphere") = {51, 72, 33};//sphere Physical Surface("front") = {38, 60, 77, 94};//front Physical Surface("back") = {17, 15, 19, 21};//back Physical Volume("interior") = {1, 2, 3, 4};//interior Cheers, Ben |
|
![]() |
![]() |
![]() |
![]() |
#2 |
Senior Member
|
Hi,
You have two kinds of warnings in your output: 1. Unhandled element type. 2. Standard "Found ... undefined faces in mesh; adding to default patch." The second should be ignored, you can find explanation of the forum. The first is caused by "2-node line" elements (type 1 in Gmsh terminology) in MSH file, which are generated due to this line: Code:
Physical Line("axis") = {6, 7, 8, 95};//ligne sym |
|
![]() |
![]() |
![]() |
![]() |
#3 |
New Member
Join Date: Jan 2017
Posts: 5
Rep Power: 9 ![]() |
Thanks for your answer!
I don't have the message "unhandled..." anymore , nevertheless I still have one problem. When I check my "boundary" file into "poly mesh", I just have 2 zone : "back" and "defaultFaces". I don't know why the other zone are not created. Do you have any idea? |
|
![]() |
![]() |
![]() |
![]() |
#4 |
Senior Member
|
Hi,
You have used wrong IDs, when defined physical surfaces. So in resulting MSH there is only physical surface 6 (back) and physical volume 7 (interior). Guess there are other faces, which do not belong to any physical surfaces and they are added to defaultFaces. |
|
![]() |
![]() |
![]() |
![]() |
#5 |
New Member
Join Date: Jan 2017
Posts: 5
Rep Power: 9 ![]() |
Hi,
Thanks, I modified something and so I forgot to change ID's. Obviously, now, I have something wrong again. When I do a checkMesh I have a fatal error : Code:
wedge wedge1 plane aligns with coordinate plane I'm sorry for all that questions but I really want to understand that axisymmetric problem. Thanks in advance, Ben. |
|
![]() |
![]() |
![]() |
![]() |
#6 |
Senior Member
|
Hi,
Wedge-type boundaries should not align with coordinate planes, so before extrusion you need to rotate plane you would like to extrude, since you have constructed geometry in X-Y plane. In general, I rotate plane by -alpha radians and then extrude by 2*alpha radians. 2*alpha should be less than 5 degrees, so usually alpha = Pi/180. |
|
![]() |
![]() |
![]() |
![]() |
#7 |
New Member
Join Date: Jan 2017
Posts: 5
Rep Power: 9 ![]() |
It's working now!
I jus have to launch some calculations now, thanks |
|
![]() |
![]() |
![]() |
Tags |
gmshtofoam problem, openfoam error |
|
|
![]() |
||||
Thread | Thread Starter | Forum | Replies | Last Post |
area does not match neighbour by ... % -- possible face ordering problem | St.Pacholak | OpenFOAM | 11 | September 4, 2024 04:28 |
Convergence Problem in Multiphase problem (three phases) | m.uzair | FLUENT | 0 | August 2, 2018 08:23 |
Large problem partitioner | tzy | CFX | 3 | February 7, 2018 17:11 |
natural convection problem for a CHT problem | Se-Hee | CFX | 2 | June 10, 2007 06:29 |
Adiabatic and Rotating wall (Convection problem) | ParodDav | CFX | 5 | April 29, 2007 19:13 |