 |
 |
 |
|
|
|
[Sponsors] | ||||
[snappyHexMesh] snappyHexMesh destroys Continuity |
9Likes
 |
|
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
July 30, 2024, 11:48
|
snappyHexMesh destroys Continuity
|
#1 |
|
New Member
Join Date: Jul 2024
Posts: 16
Rep Power: 2  |
Hello everyone,
I'm relatively new to CFD, so please excuse my rudimentary understanding. I have the following problem: I have a running two-phase simulation (interFoam, k-epsilon turbulence modelling). Now I want to extend my simulation and use SnappyHexMesh to refine my mesh depending on the location and partially cut cylinders from the mesh. I have defined boundary conditions for the newly created surfaces. Now I run my simulation as follows: blockMesh surface features snappyHexMesh -overwrite setFields interFoam Here I get the error message: --> FOAM FATAL ERROR: Continuity error cannot be removed by adjusting the outflow. Please check the velocity boundary conditions and/or run potentialFoam to initialise the outflow. Total flux : 2.22507e-308 Specified mass inflow : 2.16108e-18 Specified mass outflow : 2.2285e-18 Adjustable mass outflow : 0 Which I do not understand, because I have neither inlets nor outlets (closed system). Do you have any ideas as to why this could be? Do you need code to better understand the problem? I would be very grateful for any help. Best regards dachs |
|
|
|
|
|
August 1, 2024, 11:18
|
|
#2 |
|
Senior Member
Join Date: Dec 2021
Posts: 251
Rep Power: 5 |
Hey!
Could you post your case or at least your dictionaries used for the mesh generation? I suspect that some of your boundaries are of type patch or are not properly configured but I might be wrong. |
|
|
|
|
|
|
August 2, 2024, 03:57
|
|
#3 | |
|
New Member
Join Date: Jul 2024
Posts: 16
Rep Power: 2 |
Quote:
Hi Alczem, Sure, and Thank you for your help. Code:
/*--------------------------------*- C++ -*----------------------------------*\
| \ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \ / O peration | Version: v2312 |
| \ / A nd | Website: www.openfoam.com |
| \/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
convertToMeters 0.001;
vertices
(
(65 0 -29.0) //0
(0 65 -29.0) //1
(-65 0 -29.0) //2
(0 -65 -29.0) //3
(100 0 -29.0) //4
(0 100 -29.0) //5
(-100 0 -29.0) //6
(0 -100 -29.0) //7
(65 0 29) //8
(0 65 29) //9
(-65 0 29) //10
(0 -65 29) //11
(100 0 29) //12
(0 100 29) //13
(-100 0 29) //14
( 0 -100 29) //15
);
blocks
(
hex (1 0 4 5 9 8 12 13) (100 20 20) simpleGrading (1 1 1)
hex (2 1 5 6 10 9 13 14) (100 20 20) simpleGrading (1 1 1)
hex (3 2 6 7 11 10 14 15) (100 20 20) simpleGrading (1 1 1)
hex (0 3 7 4 8 11 15 12) (100 20 20) simpleGrading (1 1 1)
);
edges
(
arc 0 1 (45.96194077712559 45.961940777125584 -29.0)
arc 1 2 (-45.961940777125584 45.96194077712559 -29.0)
arc 2 3 (-45.9619407771256 -45.961940777125584 -29.0)
arc 3 0 (45.96194077712558 -45.9619407771256 -29.0)
arc 8 9 (45.96194077712559 45.961940777125584 29)
arc 9 10 (-45.961940777125584 45.96194077712559 29)
arc 10 11 (-45.9619407771256 -45.961940777125584 29)
arc 11 8 (45.96194077712558 -45.9619407771256 29)
arc 4 5 (67.99538807889842 67.9953880788984 -29.0)
arc 5 6 (-67.9953880788984 67.99538807889842 -29.0)
arc 6 7 (-67.99538807889843 -67.9953880788984 -29.0)
arc 7 4 (67.99538807889839 -67.99538807889843 -29.0)
arc 12 13 (67.99538807889842 67.9953880788984 29)
arc 13 14 (-67.9953880788984 67.99538807889842 29)
arc 14 15 (-67.99538807889843 -67.9953880788984 29)
arc 15 12 (67.99538807889839 -67.99538807889843 29)
);
boundary
(
innerWall
{
type wall;
faces
(
(1 0 8 9)
(2 1 9 10)
(3 2 10 11)
(0 3 11 8)
);
}
outerWall
{
type wall;
faces
(
(5 13 12 4)
(6 14 13 5)
(7 15 14 6)
(4 12 15 7)
);
}
frontWall
{
type wall;
faces
(
(8 9 12 13)
(9 10 13 14)
(10 11 14 15)
(11 8 15 12)
);
}
backWall
{
type wall;
faces
(
(0 1 4 5)
(1 2 5 6)
(2 3 6 7)
(3 0 7 4)
);
}
);
mergePatchPairs
(
);
// ************************************************************************* //
Code:
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: 7
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object snappyHexMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
castellatedMesh true;
snap true;
addLayers false;
geometry
{
middleGap
{
type triSurfaceMesh;
file "middleGap.stl";
}
innerRing
{
type triSurfaceMesh;
file "innerRing.stl";
}
outerRing
{
type triSurfaceMesh;
file "outerRing.stl";
}
roller01
{
type triSurfaceMesh;
file "roller01.stl";
}
roller02
{
type triSurfaceMesh;
file "roller02.stl";
}
roller03
{
type triSurfaceMesh;
file "roller03.stl";
}
roller04
{
type triSurfaceMesh;
file "roller04.stl";
}
roller05
{
type triSurfaceMesh;
file "roller05.stl";
}
roller06
{
type triSurfaceMesh;
file "roller06.stl";
}
roller07
{
type triSurfaceMesh;
file "roller07.stl";
}
roller08
{
type triSurfaceMesh;
file "roller08.stl";
}
roller09
{
type triSurfaceMesh;
file "roller09.stl";
}
roller10
{
type triSurfaceMesh;
file "roller10.stl";
}
roller11
{
type triSurfaceMesh;
file "roller11.stl";
}
roller12
{
type triSurfaceMesh;
file "roller12.stl";
}
roller13
{
type triSurfaceMesh;
file "roller13.stl";
}
roller14
{
type triSurfaceMesh;
file "roller14.stl";
}
roller15
{
type triSurfaceMesh;
file "roller15.stl";
}
roller16
{
type triSurfaceMesh;
file "roller16.stl";
}
roller17
{
type triSurfaceMesh;
file "roller17.stl";
}
roller18
{
type triSurfaceMesh;
file "roller18.stl";
}
roller19
{
type triSurfaceMesh;
file "roller19.stl";
}
roller20
{
type triSurfaceMesh;
file "roller20.stl";
}
rotating_inner_fluid
{
type searchableCylinder;
point1 (0.0 0.0 -0.029);
point2 (0.0 0.0 0.029);
radius 0.09616;
}
}
castellatedMeshControls
{
maxLocalCells 10000000;
maxGlobalCells 200000000;
minRefinementCells 0;
nCellsBetweenLevels 2;
maxLoadUnbalance 0.10;
features
(
{
file "innerGap.eMesh";
level 3;
}
{
file "outerGap.eMesh";
level 3;
}
{
file "middleGap.eMesh";
level 3;
}
{
file "innerRing.eMesh";
level 2;
}
{
file "outerRing.eMesh";
level 2;
}
{
file "roller01.eMesh";
level 3;
}
{
file "roller02.eMesh";
level 3;
}
{
file "roller03.eMesh";
level 3;
}
{
file "roller04.eMesh";
level 3;
}
{
file "roller05.eMesh";
level 3;
}
{
file "roller06.eMesh";
level 3;
}
{
file "roller07.eMesh";
level 3;
}
{
file "roller08.eMesh";
level 3;
}
{
file "roller09.eMesh";
level 3;
}
{
file "roller10.eMesh";
level 3;
}
{
file "roller11.eMesh";
level 3;
}
{
file "roller12.eMesh";
level 3;
}
{
file "roller13.eMesh";
level 3;
}
{
file "roller14.eMesh";
level 3;
}
{
file "roller15.eMesh";
level 3;
}
{
file "roller16.eMesh";
level 3;
}
{
file "roller17.eMesh";
level 3;
}
{
file "roller18.eMesh";
level 3;
}
{
file "roller19.eMesh";
level 3;
}
{
file "roller20.eMesh";
level 3;
}
);
resolveFeatureAngle 30;
refinementSurfaces
{
rotating_inner_fluid
{
level (1 1);
cellZone rotating_inner_fluid;
faceZone rotating_inner_fluid;
cellZoneInside inside;
}
innerGap
{
level (2 2);
}
outerGap
{
level (2 2);
}
middleGap
{
level (2 2);
}
roller01
{
level (2 2);
}
roller02
{
level (2 2);
}
roller03
{
level (2 2);
}
roller04
{
level (2 2);
}
roller05
{
level (2 2);
}
roller06
{
level (2 2);
}
roller07
{
level (2 2);
}
roller08
{
level (2 2);
}
roller09
{
level (2 2);
}
roller10
{
level (2 2);
}
roller11
{
level (2 2);
}
roller12
{
level (2 2);
}
roller13
{
level (2 2);
}
roller14
{
level (2 2);
}
roller15
{
level (2 2);
}
roller16
{
level (2 2);
}
roller17
{
level (2 2);
}
roller18
{
level (2 2);
}
roller19
{
level (2 2);
}
roller20
{
level (2 2);
}
innerRing
{
level (2 2);
}
outerRing
{
level (2 2);
}
}
refinementRegions
{
rotating_inner_fluid
{
mode inside;
levels ((1E15 1));
}
}
locationInMesh (0.012 0.0926 -0.020); // Inside point
allowFreeStandingZoneFaces false;
}
// Settings for the snapping.
snapControls
{
nSmoothPatch 3;
tolerance 1.0;
nSolveIter 300;
nRelaxIter 10;
nFeatureSnapIter 10;
implicitFeatureSnap true;
explicitFeatureSnap false;
multiRegionFeatureSnap true;
}
// Settings for the layer addition.
addLayersControls
{
relativeSizes true;
layers
{
}
expansionRatio 1.0;
finalLayerThickness 0.3;
minThickness 0.01;
nGrow 0;
featureAngle 30;
nRelaxIter 5;
nSmoothSurfaceNormals 1;
nSmoothNormals 3;
nSmoothThickness 10;
maxFaceThicknessRatio 0.5;
maxThicknessToMedialRatio 0.3;
minMedianAxisAngle 90;
nBufferCellsNoExtrude 0;
nLayerIter 50;
nRelaxedIter 20;
}
meshQualityControls
{
#include "meshQualityDict"
relaxed
{
maxNonOrtho 75;
}
}
writeFlags
(
);
mergeTolerance 1E-6;
// ************************************************************************* //
Code:
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: 7
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object meshQualityDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
//- Maximum non-orthogonality allowed. Set to 180 to disable.
maxNonOrtho 65;
//- Max skewness allowed. Set to <0 to disable.
maxBoundarySkewness 20;
maxInternalSkewness 4;
//- Max concaveness allowed. Is angle (in degrees) below which concavity
// is allowed. 0 is straight face, <0 would be convex face.
// Set to 180 to disable.
maxConcave 80;
//- Minimum pyramid volume. Is absolute volume of cell pyramid.
// Set to a sensible fraction of the smallest cell volume expected.
// Set to very negative number (e.g. -1E30) to disable.
minVol 1e-13;
//- Minimum quality of the tet formed by the face-centre
// and variable base point minimum decomposition triangles and
// the cell centre. Set to very negative number (e.g. -1E30) to
// disable.
// <0 = inside out tet,
// 0 = flat tet
// 1 = regular tet
minTetQuality 1e-15;
//- Minimum face area. Set to <0 to disable.
minArea -1;
//- Minimum face twist. Set to <-1 to disable. dot product of face normal
// and face centre triangles normal
minTwist 0.02;
//- Minimum normalised cell determinant. This is the determinant of all
// the areas of internal faces. It is a measure of how much of the
// outside area of the cell is to other cells. The idea is that if all
// outside faces of the cell are 'floating' (zeroGradient) the
// 'fixedness' of the cell is determined by the area of the internal faces.
// 1 = hex, <= 0 = folded or flattened illegal cell
minDeterminant 0.001;
//- Relative position of face in relation to cell centres (0.5 for orthogonal
// mesh) (0 -> 0.5)
minFaceWeight 0.05;
//- Volume ratio of neighbouring cells (0 -> 1)
minVolRatio 0.01;
//- Per triangle normal compared to average normal. Like face twist
// but now per (face-centre decomposition) triangle. Must be >0 for Fluent
// compatibility
minTriangleTwist -1;
nSmoothScale 4;
errorReduction 0.75;
//- If >0 : preserve cells with all points on the surface if the
// resulting volume after snapping (by approximation) is larger than
// minVolCollapseRatio times old volume (i.e. not collapsed to flat cell).
// If <0 : delete always.
//minVolCollapseRatio 0.1;
// ************************************************************************* //
|
||
|
|
|
||
|
August 2, 2024, 05:48
|
|
#4 |
|
Senior Member
Join Date: Dec 2021
Posts: 251
Rep Power: 5 |
Hey!
I can't see any obvious issue. Can you also share the resulting boundary file in polyMesh and your boundary conditions ? Is this a multiregion case or you simply needed a moving cellzone? |
|
|
|
|
|
|
August 2, 2024, 06:06
|
|
#5 |
|
Senior Member
M
Join Date: Dec 2017
Posts: 703
Rep Power: 13 |
||
|
|
|
|
|
August 2, 2024, 06:08
|
|
#6 | |
|
New Member
Join Date: Jul 2024
Posts: 16
Rep Power: 2 |
Quote:
Sure here you go: Code:
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: 11
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
format ascii;
class polyBoundaryMesh;
location "constant/polyMesh";
object boundary;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
29
(
innerWall
{
type wall;
inGroups List<word> 1(wall);
nFaces 0;
startFace 4700032;
}
outerWall
{
type wall;
inGroups List<word> 1(wall);
nFaces 0;
startFace 4700032;
}
frontWall
{
type wall;
inGroups List<word> 1(wall);
nFaces 35292;
startFace 4700032;
}
backWall
{
type wall;
inGroups List<word> 1(wall);
nFaces 35292;
startFace 4735324;
}
middleGap
{
type wall;
inGroups List<word> 1(wall);
nFaces 8480;
startFace 4770616;
}
innerRing
{
type wall;
inGroups List<word> 1(wall);
nFaces 117462;
startFace 4779096;
}
outerRing
{
type wall;
inGroups List<word> 1(wall);
nFaces 143168;
startFace 4896558;
}
roller01
{
type wall;
inGroups List<word> 1(wall);
nFaces 25204;
startFace 5039726;
}
roller02
{
type wall;
inGroups List<word> 1(wall);
nFaces 25881;
startFace 5064930;
}
roller03
{
type wall;
inGroups List<word> 1(wall);
nFaces 26005;
startFace 5090811;
}
roller04
{
type wall;
inGroups List<word> 1(wall);
nFaces 26282;
startFace 5116816;
}
roller05
{
type wall;
inGroups List<word> 1(wall);
nFaces 25903;
startFace 5143098;
}
roller06
{
type wall;
inGroups List<word> 1(wall);
nFaces 22352;
startFace 5169001;
}
roller07
{
type wall;
inGroups List<word> 1(wall);
nFaces 19668;
startFace 5191353;
}
roller08
{
type wall;
inGroups List<word> 1(wall);
nFaces 20870;
startFace 5211021;
}
roller09
{
type wall;
inGroups List<word> 1(wall);
nFaces 20868;
startFace 5231891;
}
roller10
{
type wall;
inGroups List<word> 1(wall);
nFaces 19666;
startFace 5252759;
}
roller11
{
type wall;
inGroups List<word> 1(wall);
nFaces 19180;
startFace 5272425;
}
roller12
{
type wall;
inGroups List<word> 1(wall);
nFaces 19668;
startFace 5291605;
}
roller13
{
type wall;
inGroups List<word> 1(wall);
nFaces 20870;
startFace 5311273;
}
roller14
{
type wall;
inGroups List<word> 1(wall);
nFaces 20868;
startFace 5332143;
}
roller15
{
type wall;
inGroups List<word> 1(wall);
nFaces 19665;
startFace 5353011;
}
roller16
{
type wall;
inGroups List<word> 1(wall);
nFaces 19180;
startFace 5372676;
}
roller17
{
type wall;
inGroups List<word> 1(wall);
nFaces 22878;
startFace 5391856;
}
roller18
{
type wall;
inGroups List<word> 1(wall);
nFaces 26273;
startFace 5414734;
}
roller19
{
type wall;
inGroups List<word> 1(wall);
nFaces 26268;
startFace 5441007;
}
roller20
{
type wall;
inGroups List<word> 1(wall);
nFaces 25920;
startFace 5467275;
}
inner_fluid
{
type wall;
inGroups List<word> 1(wall);
nFaces 0;
startFace 5493195;
}
inner_fluid_slave
{
type wall;
inGroups List<word> 1(wall);
nFaces 0;
startFace 5493195;
}
)
// ************************************************************************* //
Last edited by dachs; August 2, 2024 at 06:14. Reason: mistake |
||
|
|
|
||
|
August 2, 2024, 06:11
|
|
#7 | |
|
New Member
Join Date: Jul 2024
Posts: 16
Rep Power: 2 |
Quote:
Thank you for your reply, but my problem is that I have neither an inlet nor an outlet. I have a closed system so I cannot adjust the outlet BC. |
||
|
|
|
||
|
August 2, 2024, 06:32
|
|
#8 |
|
Senior Member
Join Date: Dec 2021
Posts: 251
Rep Power: 5 |
Hey,
Can you also share your boundary conditions in the 0 folder? Maybe share the whole case at this point  I noticed you have some patches with 0 faces in it, is that expected? |
|
|
|
|
|
|
August 2, 2024, 10:58
|
|
#9 | |
|
New Member
Join Date: Jul 2024
Posts: 16
Rep Power: 2 |
Quote:
Hi I had some problems sharing the whole file here but you can download it here. Thanks for your continued help. https://gigamove.rwth-aachen.de/de/d...de8a434d290554 The patches with 0 faces are not intentional. I'll have to have a look at where exactly they are created. They are probably leftovers from old code |
||
|
|
|
||
|
August 3, 2024, 07:03
|
|
#10 |
|
Senior Member
Yann
Join Date: Apr 2012
Location: France
Posts: 1,236
Rep Power: 29 |
Hello,
I am not sure this is the source of your error, but you should not use zeroGradient BCs on walls for p_rgh. Use fixedFluxPressure instead. I know using zeroGradient on pressure for solvers using gravity leads to flux calculation issues (for instance getting mass fluxes through walls). This could explain why you get continuity issues on a close system. Also, I don't think you need a p file with interFoam, and if you do, I think the BCs should be set to calculated. Probably worth trying. Yann |
|
|
|
|
|
|
August 5, 2024, 06:00
|
|
#11 | |
|
New Member
Join Date: Jul 2024
Posts: 16
Rep Power: 2 |
Quote:
Thank you for your input. Unfortunately, I still get the same error message. I personally have the feeling that it is due to snappyHExMeshDict. When I run blockMesh, setFields, InterFoam, the simulation runs normally  ....
|
||
|
|
|
||
|
August 5, 2024, 07:04
|
|
#12 |
|
Senior Member
Yann
Join Date: Apr 2012
Location: France
Posts: 1,236
Rep Power: 29 |
Have you checked your mesh after running snappy? Do you get the expected mesh?
|
|
|
|
|
|
|
August 5, 2024, 07:37
|
|
#13 | |
|
New Member
Join Date: Jul 2024
Posts: 16
Rep Power: 2 |
Quote:
Yes, I have. I use the identical mesh for a single-phase simulation with simpleFOAM. I have no problems here. I did a checkMesh and got: Code:
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time
Create polyMesh for time = 0
Time = 0s
Mesh stats
points: 5523675
faces: 14363403
internal faces: 12953887
cells: 4426076
faces per cell: 6.1719
boundary patches: 27
point zones: 0
face zones: 1
cell zones: 1
Overall number of cells of each type:
hexahedra: 3911809
prisms: 199787
wedges: 0
pyramids: 0
tet wedges: 112
tetrahedra: 0
polyhedra: 314368
Breakdown of polyhedra by number of faces:
faces number of cells
4 118
5 4978
6 54696
7 3660
8 306
9 187449
10 1926
11 16
12 53399
15 7526
18 294
Checking topology...
Boundary definition OK.
Cell to face addressing OK.
Point usage OK.
Upper triangular ordering OK.
Face vertices OK.
Number of regions: 1 (OK).
Checking patch topology for multiply connected surfaces...
Patch Faces Points Surface topology
frontWall 72076 75648 ok (non-closed singly connected)
backWall 72070 75642 ok (non-closed singly connected)
innerGap 14932 21035 ok (non-closed singly connected)
outerGap 19729 26701 ok (non-closed singly connected)
middleGap 18292 24294 ok (non-closed singly connected)
innerRing 236526 243193 ok (non-closed singly connected)
outerRing 246872 254032 ok (non-closed singly connected)
roller01 36984 38472 ok (non-closed singly connected)
roller02 38169 39651 ok (non-closed singly connected)
roller03 39356 40986 ok (non-closed singly connected)
roller04 39254 40770 ok (non-closed singly connected)
roller05 38255 39748 ok (non-closed singly connected)
roller06 35776 36804 ok (non-closed singly connected)
roller07 34743 35316 ok (non-closed singly connected)
roller08 35397 35989 ok (non-closed singly connected)
roller09 35407 35993 ok (non-closed singly connected)
roller10 34734 35307 ok (non-closed singly connected)
roller11 33749 34317 ok (non-closed singly connected)
roller12 34744 35317 ok (non-closed singly connected)
roller13 35397 35988 ok (non-closed singly connected)
roller14 35401 35988 ok (non-closed singly connected)
roller15 34737 35309 ok (non-closed singly connected)
roller16 33750 34318 ok (non-closed singly connected)
roller17 36560 37593 ok (non-closed singly connected)
roller18 39119 40627 ok (non-closed singly connected)
roller19 39224 40734 ok (non-closed singly connected)
roller20 38263 39761 ok (non-closed singly connected)
Checking geometry...
Overall domain bounding box (-0.0961497 -0.0961497 -0.029) (0.0961508 0.0961508 0.029)
Mesh has 3 geometric (non-empty/wedge) directions (1 1 1)
Mesh has 3 solution (non-empty) directions (1 1 1)
Boundary openness (1.95169e-16 -8.66665e-16 4.15461e-16) OK.
Max cell openness = 4.27151e-16 OK.
Max aspect ratio = 13.1184 OK.
Minimum face area = 1.17208e-09. Maximum face area = 6.57393e-07. Face area magnitudes OK.
Min volume = 2.52737e-13. Max volume = 3.18051e-10. Total volume = 0.000360804. Cell volumes OK.
Mesh non-orthogonality Max: 64.9997 average: 10.2477
Non-orthogonality check OK.
Face pyramids OK.
***Max skewness = 13.8247, 29 highly skew faces detected which may impair the quality of the results
<<Writing 29 skew faces to set skewFaces
Coupled point location match (average 0) OK.
Failed 1 mesh checks.
End
Last edited by dachs; August 5, 2024 at 10:19. Reason: Adding Information |
||
|
|
|
||
|
August 6, 2024, 03:59
|
|
#14 |
|
New Member
Join Date: Jul 2024
Posts: 16
Rep Power: 2 |
OK, I have customised my mesh so that the mesh check runs without errors. I still get the same error message for InterFoam
|
|
|
|
|
|
|
August 6, 2024, 07:04
|
|
#15 |
|
Senior Member
Join Date: Dec 2021
Posts: 251
Rep Power: 5 |
Hey!
After trying to run your case, I think the main issue is the geometry itself: there are tangent boundaries that create disconnected and weird-looking regions. I am pretty sure OpenFoam is not happy about this. I would try to make the geometry more "simple" to mesh, and to make sure the rollers are not touching each other especially with the rotating velocity condition they have. Regarding the contact between the rollers and the surrounding walls, you could widen a bit the enclosure and put rectangular blocks serving as contact points to avoir sharp corners. EDIT: or you can also decrease the rollers' radius I guess |
|
|
|
|
|
|
August 6, 2024, 08:49
|
|
#16 | |
|
New Member
Join Date: Jul 2024
Posts: 16
Rep Power: 2 |
Quote:
Hi, thanks again for your input. I took a closer look at the mesh today and came across this problem as well. To be honest, I don't know where these separate areas come from, as they didn't appear in older simulations. The rollers don't touch each other either, but are separated by unmoving plates (gaps). I'm really sorry that I uploaded a faulty mesh that you have now invested time in. I have restored the mesh to the "correct" old state, but I still get the same error message when running InterFoam. With checkMesh I get: Mesh ok but with checkMesh -allGeometry -allTopology I get three errors. I have cells with small quality or negative volume, cells with small determinant and many concave cells. I think the problem of continuity can occur mainly due to the cells with negative volume. I am now trying to improve the mesh and then run the simulation again. I would like to thank you and Yann again for all the input 
|
||
|
|
|
||
|
August 6, 2024, 09:04
|
|
#17 |
|
Senior Member
Join Date: Dec 2021
Posts: 251
Rep Power: 5 |
No worries
 Maybe start over from a simpler case, for instance with only one roller "floating' in a cubic domain to validate your setup and make sure the mesh is ok. It can be helpful to pinpoint the issue. Good luck!
|
|
|
|
|
|
|
August 15, 2024, 08:52
|
|
#18 |
|
New Member
Join Date: Jul 2024
Posts: 16
Rep Power: 2 |
After rebuilding the model and a lot of trial and error, I have finally fixed the problem. A little message for posterity: The biggest problem wasn't the poor mesh quality, but really the boundary conditions in 0/U. I previously used simpleFoam and here I chose the edge condition for the moving walls:
Code:
outerRing
{
type rotatingWallVelocity;
origin (0 0 0);
axis (0 0 1);
omega constant -13.325;
}
but for interFoam this does not work. Here, the speed must be defined as follows: Code:
outerRing
{
type movingWallVelocity;
value uniform (0 0 0);
velocity (0 0 0);
omega (0 0 omegaZ)
origin (0 0 0);
axis (0 0 1);
}
Last edited by dachs; August 15, 2024 at 11:25. Reason: Tipo |
|
|
|
|
|
|
| Tags |
| continuity error, interfoam solver, snappy hex mesh |
|
|
Similar Threads
|
||||
| Thread | Thread Starter | Forum | Replies | Last Post |
| pimpleDyMFoam computation randomly stops | babapeti | OpenFOAM Running, Solving & CFD | 5 | January 24, 2018 06:28 |
| How to write k and epsilon before the abnormal end | xiuying | OpenFOAM Running, Solving & CFD | 8 | August 27, 2013 16:33 |
| Upgraded from Karmic Koala 9.10 to Lucid Lynx10.04.3 | bookie56 | OpenFOAM Installation | 8 | August 13, 2011 05:03 |
| IcoFoam parallel woes | msrinath80 | OpenFOAM Running, Solving & CFD | 9 | July 22, 2007 03:58 |
| Could anybody help me see this error and give help | liugx212 | OpenFOAM Running, Solving & CFD | 3 | January 4, 2006 19:07 |
Linear Mode
