 |
 |
 |
|
|
|
[Sponsors] | ||||
SimpleFoam Diverge on Coil HeatExchanger Tank |
 |
|
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
May 2, 2020, 16:24
|
SimpleFoam Diverge on Coil HeatExchanger Tank
|
#1 |
|
New Member
Lionel Ivan
Join Date: May 2020
Location: Argentina, Buenos Aires
Posts: 2
Rep Power: 0  |
Hello Foamers,
I've experimenting converge problems with SimpleFoam, my intention is to run a Forced Heat Convection Case (FCTest), at first with a variation of tutorial's room "movingFanInRoom". As it had multiple problems, I re-wrote all the case in a new type of problem: a coil heat exchange tank. Schematically something like: Tube Coil Heat Exchanger schematic - Image With FreeCAD, I build some kind of version for my new case: FCTest-3 Body Like - Image Check Mesh give me: Code:
/*---------------------------------------------------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: 7
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
Build : 7-1ff648926f77
Exec : checkMesh
Date : May 02 2020
Time : 17:03:56
Host : "3ece253b8250"
PID : 366
I/O : uncollated
Case : /home/openfoam/run/FCTest-3
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 10)
allowSystemOperations : Allowing user-supplied system call operations
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time
Create polyMesh for time = 0
Time = 0
Mesh stats
points: 1793428
faces: 4953396
internal faces: 4722081
cells: 1582927
faces per cell: 6.1124
boundary patches: 4
point zones: 0
face zones: 0
cell zones: 0
Overall number of cells of each type:
hexahedra: 1499468
prisms: 3566
wedges: 0
pyramids: 0
tet wedges: 8
tetrahedra: 0
polyhedra: 79885
Breakdown of polyhedra by number of faces:
faces number of cells
4 6538
5 7291
6 7064
9 51660
12 6368
15 964
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
inLet 248 287 ok (non-closed singly connected)
outLet 574 597 ok (non-closed singly connected)
conteiner2 162660 162769 ok (non-closed singly connected)
helice-3 67833 77515 ok (closed singly connected)
Checking geometry...
Overall domain bounding box (0.00299734 0.00299863 0.00299783) (0.297003 0.200038 0.503003)
Mesh has 3 geometric (non-empty/wedge) directions (1 1 1)
Mesh has 3 solution (non-empty) directions (1 1 1)
Boundary openness (-9.65822e-17 -6.47508e-16 5.6816e-16) OK.
Max cell openness = 3.58514e-16 OK.
Max aspect ratio = 10.7391 OK.
Minimum face area = 2.77567e-07. Maximum face area = 2.19009e-05. Face area magnitudes OK.
Min volume = 6.26419e-10. Max volume = 5.67002e-08. Total volume = 0.0277642. Cell volumes OK.
Mesh non-orthogonality Max: 64.9115 average: 8.08358
Non-orthogonality check OK.
Face pyramids OK.
Max skewness = 3.93848 OK.
Coupled point location match (average 0) OK.
Mesh OK.
End
Here's how case mesh looks like - image When I run simpleFoam at first instance to check that flows goes fine, k grows up (blows up) from time 9 to 13 approximately when Foam experiments floating point exception. K max initially is around 2.27e0 but then jumps above 5e+68. I analysed results with paraFoam and found a singularity point (see image1 or image2) where flows accelerates x2 approximately without a physical reason. Then the acceleration expands to all container like a bomb, and also K. I made a few cuts of that region (you can see image gallery). I think that is a kind of mistake with wall calculations because I've got same singularity in my previous case (the room) also in a wall corner. I'm investigating Convergent factors, but I'm really new in CFD and also OpenFoam, so probably there is something that I'm not seeing right now. I change my relaxation factors (lower), and decrease my time step. It works better, i could reach T=14 but still having the same problem. Here's my last fvSchemes and fvSolution code: Code:
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 4.x |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
solvers
{
p_rgh
{
solver GAMG;
tolerance 1e-7; //antes -7
relTol 0.01;
smoother DICGaussSeidel;
}
p
{
solver GAMG;
tolerance 1e-06; //antes -6
relTol 0.01;
smoother GaussSeidel;
}
"(U|k|epsilon|h)"
{
solver smoothSolver;
smoother symGaussSeidel;
tolerance 1e-05; //antes -5
relTol 0.01;
}
}
SIMPLE
{
nNonOrthogonalCorrectors 0;
consistent yes;
residualControl
{
p 1e-2;
U 1e-3;
"(k|epsilon|omega|f|v2)" 1e-3;
}
pRefCell 0;
pRefValue 0;
}
relaxationFactors
{
equations
{
U 0.7; // 0.9 is more stable but 0.95 more convergent
k 0.7;
epsilon 0.7;
".*" 0.7; // 0.9 is more stable but 0.95 more convergent
}
}
// ************************************************************************* //
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 4.x |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object fvSchemes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
ddtSchemes
{
default steadyState;
}
gradSchemes
{
default Gauss linear;
}
divSchemes
{
default none;
div(phi,U) bounded Gauss linearUpwind grad(U);
div(phi,k) bounded Gauss limitedLinear 1;
div(phi,epsilon) bounded Gauss limitedLinear 1;
div(phi,K) bounded Gauss upwind;
div(phi,h) bounded Gauss upwind; //limitedLinear 0.2
// div(phi,omega) bounded Gauss limitedLinear 1;
// div(phi,v2) bounded Gauss limitedLinear 1;
div((nuEff*dev2(T(grad(U))))) Gauss linear;
div(((rho*nuEff)*dev2(T(grad(U))))) Gauss linear;
div(nonlinearStress) Gauss linear;
}
laplacianSchemes
{
default Gauss linear corrected;
}
interpolationSchemes
{
default linear;
}
snGradSchemes
{
default corrected;
}
wallDist
{
method meshWave;
}
// ************************************************************************* //
All case files you can find in this link. Error Log is here. I'll appreciate all kind of help or advices, Thanks you in advance
__________________
Eng. Lionel Ivan Last edited by Lionel Ivan; May 3, 2020 at 10:00. |
|
|
|
|
|
May 9, 2020, 13:36
|
|
#2 |
|
Senior Member
Herpes Free Engineer
Join Date: Sep 2019
Location: The Home Under The Ground with the Lost Boys
Posts: 931
Rep Power: 13 |
Hi,
- Could you please execute the following to obtain a more detailed mesh quality info: Code:
checkMesh -allGeometry -allTopology -latestTime - Sometimes, the kEpsilon closure model becomes numerically unstable for the initial steps even though every setting is plausible. Few suggestions: - Change "gradSchemes" of velocity from: Code:
gradSchemes
{
default Gauss linear;
}
Code:
gradSchemes
{
default Gauss linear;
grad(U) cellMDLimited Gauss linear 1;
}
Code:
div(phi,k) bounded Gauss limitedLinear 1;
div(phi,epsilon) bounded Gauss limitedLinear 1;
Code:
div(phi,k) bounded Gauss upwind;
div(phi,epsilon) bounded Gauss upwind;
- Could you please try to use "kOmegaSST" instead? Hope these help.
__________________
The OpenFOAM community is the biggest contributor to OpenFOAM: User guide/Wiki-1/Wiki-2/Code guide/Code Wiki/Journal Nilsson/Guerrero/Holzinger/Holzmann/Nagy/Santos/Nozaki/Jasak/Primer Governance Bugs/Features: OpenFOAM (ESI-OpenCFD-Trademark) Bugs/Features: FOAM-Extend (Wikki-FSB) Bugs: OpenFOAM.org How to create a MWE New: Forkable OpenFOAM mirror |
|
|
|
|
|
|
May 9, 2020, 19:03
|
|
#3 |
|
New Member
Lionel Ivan
Join Date: May 2020
Location: Argentina, Buenos Aires
Posts: 2
Rep Power: 0 |
Hey HPE, thanks you for your reply! It's really useful for me.
Here I copy the output of CheckMesh Command: Code:
/*---------------------------------------------------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: 7
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
Build : 7-1ff648926f77
Exec : checkMesh -allGeometry -allTopology -latestTime
Date : May 09 2020
Time : 21:45:23
Host : "13ee4b67678f"
PID : 202
I/O : uncollated
Case : /home/openfoam/run/FCTest-3
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 10)
allowSystemOperations : Allowing user-supplied system call operations
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time
Create polyMesh for time = 120
Enabling all (cell, face, edge, point) topology checks.
Enabling all geometry checks.
Time = 120
Mesh stats
points: 1793428
faces: 4953396
internal faces: 4722081
cells: 1582927
faces per cell: 6.1124
boundary patches: 4
point zones: 0
face zones: 0
cell zones: 0
Overall number of cells of each type:
hexahedra: 1499468
prisms: 3566
wedges: 0
pyramids: 0
tet wedges: 8
tetrahedra: 0
polyhedra: 79885
Breakdown of polyhedra by number of faces:
faces number of cells
4 6538
5 7291
6 7064
9 51660
12 6368
15 964
Checking topology...
Boundary definition OK.
Cell to face addressing OK.
Point usage OK.
Upper triangular ordering OK.
Face vertices OK.
Topological cell zip-up check OK.
Face-face connectivity OK.
Number of regions: 1 (OK).
Checking patch topology for multiply connected surfaces...
Patch Faces Points Surface topology Bounding box
inLet 248 287 ok (non-closed singly connected) (0.130049 0.199705 0.0300393) (0.17004 0.200038 0.0699604)
outLet 574 597 ok (non-closed singly connected) (0.130075 0.0300683 0.502986) (0.169955 0.0699267 0.503003)
conteiner2 162660 162769 ok (non-closed singly connected) (0.00299734 0.00299863 0.00299783) (0.297003 0.2 0.503)
helice-3 67833 77515 ok (closed singly connected) (0.0685578 0.0185422 0.0936609) (0.231468 0.181481 0.40633)
Checking geometry...
Overall domain bounding box (0.00299734 0.00299863 0.00299783) (0.297003 0.200038 0.503003)
Mesh has 3 geometric (non-empty/wedge) directions (1 1 1)
Mesh has 3 solution (non-empty) directions (1 1 1)
Boundary openness (-9.65822e-17 -6.47508e-16 5.6816e-16) OK.
Max cell openness = 3.58514e-16 OK.
Max aspect ratio = 10.7391 OK.
Minimum face area = 2.77567e-07. Maximum face area = 2.19009e-05. Face area magnitudes OK.
Min volume = 6.26419e-10. Max volume = 5.67002e-08. Total volume = 0.0277642. Cell volumes OK.
Mesh non-orthogonality Max: 64.9115 average: 8.08358
Non-orthogonality check OK.
Face pyramids OK.
Max skewness = 3.93848 OK.
Coupled point location match (average 0) OK.
Face tets OK.
Min/max edge length = 4.43851e-05 0.0061257 OK.
*There are 4977 faces with concave angles between consecutive edges. Max concave angle = 75.5406 degrees.
<<Writing 4977 faces with concave angles to set concaveFaces
Face flatness (1 = flat, 0 = butterfly) : min = 0.719631 average = 0.999484
*There are 155 faces with ratio between projected and actual area < 0.8
Minimum ratio (minimum flatness, maximum warpage) = 0.719631
<<Writing 155 warped faces to set warpedFaces
Cell determinant (wellposedness) : minimum: 0.084231 average: 7.07777
Cell determinant check OK.
***Concave cells (using face planes) found, number of cells: 41229
<<Writing 41229 concave cells to set concaveCells
Face interpolation weight : minimum: 0.128579 average: 0.484793
Face interpolation weight check OK.
Face volume ratio : minimum: 0.103903 average: 0.924498
Face volume ratio check OK.
Failed 1 mesh checks.
End
I've been investigating and decided to apply another turbulence model (I incorrectly thought that K-Epsilon would be easier for me as new user). Fortunately I had chosen KOmegaSST, and... It works! You are right! I've been running for almost 6 hours so stopped it at Time = 120. Here last log of solver: Code:
Time = 119.75
smoothSolver: Solving for Ux, Initial residual = 0.0146202, Final residual = 0.00124374, No Iterations 5
smoothSolver: Solving for Uy, Initial residual = 0.0112093, Final residual = 0.000941393, No Iterations 5
smoothSolver: Solving for Uz, Initial residual = 0.018397, Final residual = 0.00159775, No Iterations 5
smoothSolver: Solving for Ux, Initial residual = 0.014646, Final residual = 0.00125485, No Iterations 5
smoothSolver: Solving for Uy, Initial residual = 0.0111445, Final residual = 0.000943403, No Iterations 5
smoothSolver: Solving for Uz, Initial residual = 0.018326, Final residual = 0.00159918, No Iterations 5
GAMG: Solving for p, Initial residual = 0.0404628, Final residual = 0.00258905, No Iterations 2
time step continuity errors : sum local = 0.00339386, global = -1.1418e-05, cumulative = -0.00979684
GAMG: Solving for p, Initial residual = 0.0403479, Final residual = 0.00253144, No Iterations 2
time step continuity errors : sum local = 0.00332066, global = -1.16226e-05, cumulative = -0.00978542
smoothSolver: Solving for omega, Initial residual = 0.00355531, Final residual = 0.000107591, No Iterations 2
smoothSolver: Solving for k, Initial residual = 0.00909062, Final residual = 0.000515162, No Iterations 2
bounding k, min: -2.92472e-05 max: 0.0117795 average: 0.000501664
smoothSolver: Solving for omega, Initial residual = 0.00355179, Final residual = 0.000107708, No Iterations 2
smoothSolver: Solving for k, Initial residual = 0.00909774, Final residual = 0.00051932, No Iterations 2
bounding k, min: -6.34132e-05 max: 0.0117395 average: 0.00050137
ExecutionTime = 19099.2 s ClockTime = 20090 s
Time = 120
smoothSolver: Solving for Ux, Initial residual = 0.0146202, Final residual = 0.00124374, No Iterations 5
smoothSolver: Solving for Uy, Initial residual = 0.0112093, Final residual = 0.000941393, No Iterations 5
smoothSolver: Solving for Uz, Initial residual = 0.018397, Final residual = 0.00159775, No Iterations 5
GAMG: Solving for p, Initial residual = 0.0404628, Final residual = 0.00258905, No Iterations 2
time step continuity errors : sum local = 0.00339386, global = -1.1418e-05, cumulative = -0.00979684
smoothSolver: Solving for omega, Initial residual = 0.00355531, Final residual = 0.000107591, No Iterations 2
smoothSolver: Solving for k, Initial residual = 0.00909062, Final residual = 0.000515162, No Iterations 2
bounding k, min: -2.92472e-05 max: 0.0117795 average: 0.000501664
--> FOAM Warning :
From function bool Foam::rmDir(const Foam::fileName&)
in file POSIX.C at line 1069
cannot open directory ""
ExecutionTime = 19086.6 s ClockTime = 20110 s
End
--> FOAM Warning :
From function bool Foam::rmDir(const Foam::fileName&)
in file POSIX.C at line 1069
cannot open directory ""
ExecutionTime = 19130.1 s ClockTime = 20122 s
End
Now I'll try run bouyantSimpleFoam to solve heat transfer. I'll tell you if I get success. Finally, I will re-run kEpsilon model with your corrections. Thanks you again! PS: New fvSchemes and fvSolution configuration. Code:
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 4.x |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
solvers
{
p_rgh
{
solver GAMG;
tolerance 1e-7; //antes -7
relTol 0.1;
smoother DICGaussSeidel;
}
p
{
solver GAMG;
tolerance 1e-06; //antes -6
relTol 0.1;
smoother GaussSeidel;
}
"(U|k|epsilon|h|omega)"
{
solver smoothSolver;
smoother symGaussSeidel;
tolerance 1e-05; //antes -5
relTol 0.1;
}
}
SIMPLE
{
nNonOrthogonalCorrectors 0;
consistent yes;
residualControl
{
p 1e-2;
U 1e-3;
"(k|epsilon|omega|f|v2)" 1e-3;
}
pRefCell 0;
pRefValue 0;
}
relaxationFactors
{
equations
{
U 0.9; // 0.9 is more stable but 0.95 more convergent
k 0.9;
epsilon 0.9;
omega 0.9;
".*" 0.9; // 0.9 is more stable but 0.95 more convergent
}
}
// ************************************************************************* //
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 5 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object fvSchemes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
ddtSchemes
{
default steadyState;
}
gradSchemes
{
default Gauss linear;
}
divSchemes
{
default none;
div(phi,U) bounded Gauss linearUpwind grad(U);
div(phi,k) bounded Gauss limitedLinear 1;
div(phi,epsilon) bounded Gauss limitedLinear 1;
div(phi,omega) bounded Gauss limitedLinear 1;
div(phi,v2) bounded Gauss limitedLinear 1;
div((nuEff*dev2(T(grad(U))))) Gauss linear;
div(nonlinearStress) Gauss linear;
}
laplacianSchemes
{
default Gauss linear corrected;
}
interpolationSchemes
{
default linear;
}
snGradSchemes
{
default corrected;
}
wallDist
{
method meshWave;
}
// ************************************************************************* //
__________________
Eng. Lionel Ivan |
|
|
|
|
|
|
| Tags |
| divergence, kepsilon, kepsilonmodel, simplefoam, simplefoam convergence |
|
|
Similar Threads
|
||||
| Thread | Thread Starter | Forum | Replies | Last Post |
| ANSYS Fluent Sloshing in baffled tank simulation | Fisya | CFD Freelancers | 2 | August 27, 2019 18:55 |
| coil tank | yassoub | FLUENT | 0 | September 14, 2017 10:40 |
| simpleFoam parallel solver & Fluent polyhedral mesh | Zlatko | OpenFOAM Running, Solving & CFD | 3 | September 26, 2014 07:53 |
| Mixing Tank using simpleFoam - PLEASE HELP! | sbusmayer | OpenFOAM Running, Solving & CFD | 3 | October 23, 2013 19:30 |
| Emptying Tank simpleFoam | idrama | OpenFOAM | 6 | May 10, 2013 04:38 |
Linear Mode
