[stonepreston]

Hey Everyone,


I just started using OpenFOAM and am still new to CFD in general. I am trying to get the cavity tutorial working using gmsh instead of blockMesh.



Here is my .geo file

// Gmsh project created on Fri Jun 15 11:49:11 2018
SetFactory("OpenCASCADE");
//+
//+
// Define variable to control mesh refinement
h = .01;
Point(1) = {0, 0, 0, h};
//+
Point(2) = {0.1, 0, 0, h};
//+
Point(3) = {0.1, 0.1, 0,h};
//+
Point(4) = {0, 0.1, 0, h};
//+
Line(1) = {1, 2};
//+
Line(2) = {2, 3};
//+
Line(3) = {3, 4};
//+
Line(4) = {4, 1};
//+
Line Loop(1) = {3, 4, 1, 2};
//+
Plane Surface(1) = {1};
//+
Transfinite Line {3, 1, 4, 2} = 21 Using Progression 1;
//+
Transfinite Surface {1};
//+
Recombine Surface {1};
//+
//+
//+
Extrude {0, 0, .005} {
  Surface{1}; Layers{1}; Recombine;
}
//+
Physical Surface("movingWall") = {2};
//+
Physical Surface("fixedWalls") = {3, 4, 5};
//+
Physical Surface("frontAndBack") = {6, 1};
//+
Physical Volume("fluid") = {1};

The mesh is 20 x 20 cells in the xy direction and 1 cell thick in the z direction. I made sure all the physical boundary names matched those used in the original cavity tutorial. An image of my mesh is attached.



I converted the gmsh .msh file to openFoam using

gmshToFoam cavity.msh

and it created all the mesh files inside the polyMesh directory. I then modified the boundary file to match that of the original tutorial. One thing I did notice was that this boundary files has a type field AND a physicalType field. Whats the difference between the 2? Nevertheless, here is my boundary file:

FoamFile
{
    version     2.0;
    format      ascii;
    class       polyBoundaryMesh;
    location    "constant/polyMesh";
    object      boundary;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

3
(
    frontAndBack
    {
        type            empty;
        physicalType    empty;
        nFaces          800;
        startFace       760;
    }
    movingWall
    {
        type            wall;
        physicalType    wall;
        nFaces          20;
        startFace       1560;
    }
    fixedWalls
    {
        type            wall;
        physicalType    wall;
        nFaces          60;
        startFace       1580;
    }
)

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

I then ran

icoFoam

In paraFoam, my results are quite different than the original tutorial. I have attached pictures of my pressure and velocity contours. The shape of the pressure contour is correct but the numbers do not match that of the original tutorial. The shape of the velocity contour is a bit off as well.



Any ideas what is going on?



Thanks

[alexeym]

Hi,

In fact velocity fields are identical for blockMesh and Gmsh generated meshes. Absolute values of pressure are different, but it is difference, that matters/drives flow, and the difference is the same for both simulations (9.2 Pa). In fact, different distributions of pressure are caused by different locations of 0 Pa (which, by default, is in cell with ID = 0).

Since it is icoFoam and meshes are slightly different, I would not worry much about these result differences.

I ran simulations with OpenFOAM-plus 1806 pre-release. What version did you use?

[stonepreston]

Originally Posted by alexeym

Hi,

In fact velocity fields are identical for blockMesh and Gmsh generated meshes. Absolute values of pressure are different, but it is difference, that matters/drives flow, and the difference is the same for both simulations (9.2 Pa). In fact, different distributions of pressure are caused by different locations of 0 Pa (which, by default, is in cell with ID = 0).

Since it is icoFoam and meshes are slightly different, I would not worry much about these result differences.

I ran simulations with OpenFOAM-plus 1806 pre-release. What version did you use?

I used OpenFOAM-5.0

[alexeym]

Well, I do not have 5.0 installed, but still the difference in pressure distributions are caused by different mesh cells numbering (and necessity to solve Poisson equation with pure Neumann BCs).

And as a side-note: it is not quite fair to compare interpolated point fields in ParaView (real velocity, for example, is located in the cell centres, so it is cell data in terms of ParaView). Use sample function object to extract data directly from simulation.