|
[Sponsors] |
January 9, 2015, 05:01 |
Fluent works... OF not?
|
#1 | |
New Member
Angelo Ugenti
Join Date: Dec 2014
Location: Bari
Posts: 8
Rep Power: 11 |
Hi everybody,
I'm studying Mechanical Engineering at Politecnico di Bari (Italy). I'm writing a thesis analyzing incompressible flow over an airfoil. (turbulence model: k-omega; flow velocity: 20 m/s; nu=10^-4 m^2/s; rho= 1 kg/m^3) I made the mesh with Pointwise. I run it first with Fluent and it worked. I tried to run the analysis in OpenFOAM so I adapted the "motorbike" tutorial to my case. But it doesn't work. Quote:
If you need any of the case files, please ask me. |
||
January 9, 2015, 05:06 |
|
#2 |
Senior Member
|
Hi,
As the solver crashes during the first iteration, it can be mesh, schemes, ICs and BCs. So please post: 1. checkMesh output 2. fvSchemes file 3. 0 folder |
|
January 9, 2015, 06:06 |
|
#3 | ||
New Member
Angelo Ugenti
Join Date: Dec 2014
Location: Bari
Posts: 8
Rep Power: 11 |
CheckMesh
Quote:
fvSchemes Quote:
|
|||
January 9, 2015, 08:23 |
|
#4 |
Senior Member
|
Hi,
I was not able to find errors in the settings, my suggestions will be quite generic: 1. Change smoothSolver to PBiCG. Dictionary for the solver you can find in $FOAM_TUTORIALS/heatTransfer/buoyantBoussinesqPimpleFoam/hotRoom/system/fvSolution. 2. As your mesh has highly non-orthogonal faces, consider using cellMDLimited modifications of schemes for gradients. Examples can be found in $FOAM_TUTORIALS/incompressible/pisoFoam/les/motorBike/motorBike/system/fvSchemes (though not quite sure it will be there in 2.1.1, I don't have this version installed). 3. Add bounded to divergence schemes. Example can be found in $FOAM_TUTORIALS/incompressible/simpleFoam/pitzDailyExptInlet/system/fvSchemes. |
|
January 9, 2015, 17:46 |
|
#5 |
Senior Member
anonymous
Join Date: Aug 2014
Posts: 205
Rep Power: 12 |
Your does seem to be the problem. Are you sure you changed frontAndBack to empty in the boundary file?
|
|
January 10, 2015, 07:12 |
|
#6 | ||||||
New Member
Angelo Ugenti
Join Date: Dec 2014
Location: Bari
Posts: 8
Rep Power: 11 |
@alexeym
1) I changed the solver for U, k, omega from smoothSolver to PBiCG. 2) I used cellMDLimited Quote:
Quote:
Quote:
Quote:
it gaves me an error: Quote:
So I tried to run with only modifications 1 and 2. Results: Quote:
Yes, boundary conditions are ok. Any more tips? Should be the problem the GAMGSolver (which is the selected solver for p)? |
|||||||
January 10, 2015, 08:27 |
|
#7 |
Senior Member
anonymous
Join Date: Aug 2014
Posts: 205
Rep Power: 12 |
In order to use bounded in the fvSchemes you need Openfoam2.2.0 or greater, you are using of2.1.1
Are you sure your boundary conditions are correct? Maybe there is a variable whith initial value of 0 (omega...)? |
|
January 10, 2015, 08:30 |
|
#8 |
Senior Member
|
Hi,
Well, guess bounded was not implemented in 2.1.1. According to the output, this time FPE happens in pEqn.H, so you've got two options: 1. Change solver for pressure to PCG. 2. Increase number of cell in coarsest level for GAMG solver (nCellsInCoarsestLevel). In general I set this value to nCellsInMesh^(1/3) (for 2D case it could be nCellsInMesh^(1/2), so for ~100,000 cells in your mesh the value should be around 320) Also I've noticed this line in the output: Code:
SIMPLE: no convergence criteria found. Calculations will run for 500 steps. |
|
January 10, 2015, 11:14 |
|
#9 | ||||
New Member
Angelo Ugenti
Join Date: Dec 2014
Location: Bari
Posts: 8
Rep Power: 11 |
I'll download the 2.2 version as last option
@ssss omega value is 1.78 everywhere. I uploaded the 0 folder in a precedent post so you can check it. I added residualControl. I increased the number of cell in coarsest level Quote:
So I changed the GAMG solver Quote:
Quote:
Looking to last outputs I think that something went wrong Quote:
Any more tips before updating OF in order to use the bounded divSchemes? |
|||||
January 10, 2015, 12:59 |
|
#10 |
Senior Member
|
Hi,
"relTol 0" in pressure solver is too strict. Let it be 1e-2 or 0.1. Don't know what values of tolerance and relTol you have for velocity. As you can see from residuals, solution is far from convergence. Increase endTime to say 25000. If solution converge earlier, it will just stop at the point of convergence. Don't know the reason for the core dump, though as solution diverges, maybe certain values in result files lead to this behavior. Try using paraview's build-in OpenFOAM reader (paraFoam -builtin). |
|
January 10, 2015, 13:43 |
|
#11 | ||
New Member
Angelo Ugenti
Join Date: Dec 2014
Location: Bari
Posts: 8
Rep Power: 11 |
I fixed the fvSolution file
Quote:
Results: Quote:
|
|||
January 10, 2015, 13:56 |
|
#12 |
Senior Member
|
Hi,
1. Increase number of non-orthogonal correctors. nNonOrthogonalCorrectors in SIMPLE dictionary. Set it to 3-4. 2. If solution still diverges. Relax more. Set relaxation factor for velocity to 0.3. |
|
January 12, 2015, 09:55 |
|
#13 | |
New Member
Angelo Ugenti
Join Date: Dec 2014
Location: Bari
Posts: 8
Rep Power: 11 |
I set the number of non-orthogonal correctors to 4.
Quote:
|
||
January 12, 2015, 10:19 |
|
#14 |
Senior Member
|
Hi,
If you take a look at forceCoeffs.C: Code:
// lift, drag and moment coeffs[0] = (totForce & liftDir_)/(Aref_*pDyn); coeffs[1] = (totForce & dragDir_)/(Aref_*pDyn); coeffs[2] = (totMoment & pitchAxis_)/(Aref_*lRef_*pDyn); scalar Cl = sum(coeffs[0]); scalar Cd = sum(coeffs[1]); scalar Cm = sum(coeffs[2]); |
|
January 12, 2015, 10:39 |
|
#15 |
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 26 |
Angelo please try:
Code:
p { solver GAMG; tolerance 1e-12; relTol 0.1; smoother DICGaussSeidel; nPreSweeps 0; nPostSweeps 1; nFinestSweeps 2; scaleCorrection true; directSolveCoarsestLevel false; cacheAgglomeration on; agglomerator faceAreaPair; nCellsInCoarsestLevel 500; mergeLevels 1; maxIter 100; } Code:
"(U|k|omega)" { solver smoothSolver; preconditioner DILU; smoother DILUGaussSeidel; tolerance 1e-12; relTol 0.1; nSweeps 1; maxIter 100; }
__________________
The skeleton ran out of shampoo in the shower. |
|
January 12, 2015, 10:40 |
|
#16 |
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 26 |
Also one very clever person in this forum wrote you should never limit the pressure gradient.
__________________
The skeleton ran out of shampoo in the shower. |
|
January 12, 2015, 11:03 |
|
#17 |
Senior Member
|
In fact it was here: http://www.openfoam.org/mantisbt/view.php?id=1410#c3246
|
|
January 13, 2015, 01:18 |
|
#18 |
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 26 |
Right there, henry... very clever.
__________________
The skeleton ran out of shampoo in the shower. |
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Interesting problem: Parallel Processor VOF Fluent + Dynamic Mesh + System Coupling | spaceprop | FLUENT | 5 | September 2, 2014 09:43 |
The fluent stopped and errors with "Emergency: received SIGHUP signal" | yuyuxuan | FLUENT | 0 | December 3, 2013 22:56 |
What the differences flow equation of Fluent 6.3 and Fluent 12.1 | opehterinar81 | FLUENT | 0 | August 19, 2011 11:55 |
Fluent 6.3 32bit vs Fluent 12.0 64bit | ibex7 | FLUENT | 7 | April 18, 2011 02:44 |
How does a Fluent LICENCE works? | Freeman | FLUENT | 4 | April 14, 2006 05:58 |