[mmeyer]

Hello Foamers,

I'm trying to simulate combustion in a diesel engine, by copying our Kiva mesh to the combustion/engineFoam/kivaTest tutorial case.

Our mesh does not contain the whole 360° cylinder, but a "piece of cake" with cyclic boundary.

Mesh conversion runs just fine, but engineFoam can only compute crank angles from -180° to at most -178° before the velocity field at the center of the piston is getting very unstable and finally janafThermo gives the Fatal Error.

Maybe just copying a cyclic mesh to the (non-cyclic) Tutorial Case isn't enough. Can anyone help me?

Thanks in advance, Max

[mmeyer]

I am using Foam-Extend-3.1

These are my logfiles including an attempt to refine the mesh.

[mmeyer]

I edited the global controlDict in the following way:

...
DebugSwitches
  {
    cyclic  1;
    ...
  }
...
Tolerances
  {
    patchFaceMatchTol  1e-3;
    ...
  }
...

Thereby I gained almost 30° of crank angle, but in every step a Serious Error in cyclicPolyPatch occurs:

cyclicPolyPatch::calcTransforms : Writing half0 faces to file "/home/mmeyer/foam/mmeyer-3.1/run/KIVAgrid/kivaTest/VTK/cyclic_half0_faces"
cyclicPolyPatch::calcTransforms : Writing half1 faces to file "/home/mmeyer/foam/mmeyer-3.1/run/KIVAgrid/kivaTest/VTK/cyclic_half1_faces"
Unknown transform: calculating transform from geometry
--> FOAM Serious Error : 
    From function void cyclicPolyPatch::calcTransforms() const
    in file meshes/polyMesh/polyPatches/constraint/cyclic/cyclicPolyPatch.C at line 246
    Transformation tensor is not constant for the cyclic patch cyclic.  Please reconsider your setup and definition of cyclic boundaries.
cyclicPolyPatch::calcTransforms : Writing transform_half0 faces to file "/home/mmeyer/foam/mmeyer-3.1/run/KIVAgrid/kivaTest/VTK/cyclic_transform_half0_faces"

After a couple of these, Foam aborts because of "Too many errors"

[mmeyer]

My latest approach is to define the unknown transformation tensor by hand, but I don't know if the faceSets are created and named properly by the kivaToFoam tool.

[tsencic]

I am trying to simulate a diesel engine using a sector of 51 degree mesh.
I use the foam-extend-3.1 version. The mesh is created with blockMesh.

I obtain the error
--> FOAM FATAL ERROR:
face 2 area does not match neighbour 5 by 179.301% -- possible face ordering problem.
patch:front my area:155.763 neighbour area:2854.34 matching tolerance:0.0001
Mesh face:19 vertices:4((15.4535 -7.43725 -13.65) (22.0764 -10.6246 -19.5) (28.2262 -13.5844 0) (19.7584 -9.50906 0))
Neighbour face:22 vertices:4((28.2262 -13.5844 0) (48.6582 -23.4176 0) (48.6582 -23.4176 125.88) (28.2262 -13.5844 125.88))
Other errors also exist, only the largest is reported. Please rerun with cyclic debug flag set for more information.


This is my blockMeshDict file:
/*--------------------------------------------------------------------------*
| ========= | |
| \ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \ / O peration | Version: 1.0 |
| \ / A nd | Web: http://www.openfoam.org |
| \/ M anipulation | |
*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
root ;
case ;
instance ;
local ;
class dictionary;
object blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
convertToMeters 0.001;
vertices

(
(0.973163 -0.468352 -17.8) //0
(22.0764 -10.6246 -19.5) //1
(22.0764 10.6246 -19.5) //2
(0.973163 0.468352 -17.8) //3
(0.973163 -0.468352 0) //4
(28.2262 -13.5844 0) //5
(48.6582 -23.4176 0) //6
(48.6582 23.4176 0) //7
(28.2262 13.5844 0) //8
(0.973163 0.468352 0) //9
(0.973163 -0.468352 125.88) //10
(28.2262 -13.5844 125.88) //11
(48.6582 -23.4176 125.88) //12
(48.6582 23.4176 125.88) //13
(28.2262 13.5844 125.88) //14
(0.973163 0.468352 125.88) //15
(15.4535 -7.43725 -13.65) //16
(15.4535 7.43725 -13.65) //17
(19.7584 -9.50906 0) //18
(19.7584 9.50906 0) //19
(19.7584 -9.50906 125.88) //20
(19.7584 9.50906 125.88) //21
(0.973163 -0.468352 -8.9) //22
(0.973163 0.468352 -8.9) //23
);

blocks
(
hex (0 1 2 3 22 16 17 23) (10 25 6) simpleGrading (1 1 1)
hex (22 16 17 23 4 18 19 9) (10 25 14) simpleGrading (1 1 1)
hex (16 1 2 17 18 5 8 19) (6 25 14) simpleGrading (1 1 1)
hex (4 18 19 9 10 20 21 15) (10 25 26) simpleGrading (1 1 1)
hex (18 5 8 19 20 11 14 21) (6 25 26) simpleGrading (1 1 1)
hex (5 6 7 8 11 12 13 14) (16 25 26) simpleGrading (1 1 1)
);

edges
(
arc 0 3 (1.08 0 -17.8)
arc 1 2 (24.5 0 -19.5)
arc 4 9 (1.08 0 0)
arc 5 8 (31.325 0 0)
arc 6 7 (54 0 0)
arc 10 15 (1.08 0 125.88)
arc 11 14 (31.325 0 125.88)
arc 12 13 (54 0 125.88)
arc 22 23 (1.08 0 -8.9)
arc 16 17 (17.15 0 -13.65)
arc 18 19 (21.9275 0 0)
arc 20 21 (21.9275 0 125.88)
spline 0 1( (4.50539 -2.1683 -19) (9.01077 -4.33659 -20) (16.2194 -7.80586 -21) )
spline 3 2( (4.50539 2.1683 -19) (9.01077 4.33659 -20) (16.2194 7.80586 -21) )
spline 1 5( (28.2262 -13.5844 -11) )
spline 2 8( (28.2262 13.5844 -11) )
);

patches
(
wall
piston
(
( 0 1 2 3)
( 1 2 8 5)
(5 6 7 8)
)
wall
liner
(
( 6 12 13 7)
)
wall
cylinderHead
(
( 10 20 21 15)
( 20 11 14 21)
( 11 12 13 14)
)
symmetryPlane
symmetryFaces
(
( 0 22 23 3)
( 22 4 9 23)
( 4 10 15 9)
)
cyclic
front
(
( 0 1 16 22)
( 22 16 18 4)
( 16 1 5 18 )
( 4 18 20 10)
( 18 5 11 20)
( 5 6 12 11)
)

cyclic
back
(
( 3 23 17 2)
( 23 9 19 17)
( 17 19 8 2)
( 9 15 21 19)
( 19 21 14 8)
( 8 14 13 7)
)
);

mergePatchPairs ();
// ************************************************** *********************** //

I also tried to have one cyclic boundary, frontAndBack, then I get:

--> FOAM Serious Error :
From function void cyclicPolyPatch::calcTransforms() const
in file meshes/polyMesh/polyPatches/constraint/cyclic/cyclicPolyPatch.C at line 246
Transformation tensor is not constant for the cyclic patch frontAndBack. Please reconsider your setup and definition of cyclic boundaries.

I remember that I used this kind of mesh on earlier OF versions, like OF-1.4 and 1.5. It should be a simple thing, this is not a complex geometry and is similar for many engine applications, but I see many have problems with cyclics :-(
How could I solve the problem?

[mmeyer]

--> FOAM FATAL ERROR:
face 2 area does not match neighbour 5 by 179.301% -- possible face ordering problem.

So, you use rotational cyclic boundaries, too (?). The error above could be related to the transformation tensor. In order to simulate a 51° sector of the cylinder, I had to define a 309° transformation tensor in ./constant/polyMesh/boundary:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | foam-extend: Open Source CFD                    |
|  \\    /   O peration     | Version:     3.1                                |
|   \\  /    A nd           | Web:         http://www.extend-project.de       |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       polyBoundaryMesh;
    location    "constant/polyMesh";
    object      boundary;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

4
(
    piston
    {
        type            wall;
        nFaces          2140;
        startFace       165197;
    }
    liner
    {
        type            wall;
        nFaces          460;
        startFace       167337;
    }
    cylinderHead
    {
        type            wall;
        nFaces          1700;
        startFace       167797;
    }
    cyclic
    {
        type            cyclic;
        nFaces          5686;
        startFace       169497;
        featureCos      0.9;
        transform       rotational;
        rotationAxis    (0 0 1);
        rotationCentre  (0 0 0);
        rotationAngle   308.571;
    }
)

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

[tsencic]

Thank You very much. It's working now.

[zhouqy1994]

Hi mmeyer

I am facing the same problem now...

When using a sector for simulation, the velocity in the center of piston is unstable.

Have you got the solutions or any tips?

I am really confused by that

Thanks in advance


Sent from my iPhone using CFD Online Forum mobile app

[zhouqy1994]

my simulation runs fine from -180--146,and then the velocity becomes really high and then janafThermo out of range

Any advice is welcome

Thanks in advance


Sent from my iPhone using CFD Online Forum mobile app