|
[Sponsors] |
January 18, 2012, 12:22 |
Boundary Conditions in rhoSimplecFoam
|
#1 |
New Member
Join Date: Oct 2011
Posts: 20
Rep Power: 15 |
Hello friends,
I am trying to make a turbulent flow simulation with using rhoSimplecFoam ver. OpenFOAM-2.1.0. When I run my case after 12 iteration I get an error message. After spending lots of time and many attempts I decided to open a tread in forum. Could someone help me where is the mistake in my boundary conditions? If someone corrects my BCs, that tread can be an example for other foamers. Inlet P : totalPressure U : pressureDirectedInletVelocity T : fixedValue k : fixedValue mut : fixedValue epsilon : compressible::turbulentMixingLengthDissipationRate Inlet alphat : fixedValue Outlet P : fixedValue U : zeroGradient T : fixedValue k :zeroGradient mut : zeroGradient epsilon : fixedValue alphat : fixedValue FixedWalls P : zeroGradient U : fixedValue (0 0 0) T : zeroGradient k : compressible::kqRWallFunction mut : mutkWallFunction epsilon : compressible::epsilonWallFunction alphat : alphatWallFunction Left cyclic Right cyclic I do not know exact outlet pressure. But I can make a good guess for it. My velocities are low and at the outlet they must be slower than the inlet. I can guess it from the formula of total pressure. Thanks in advance! Regards Gökhan |
|
March 5, 2012, 11:47 |
|
#2 |
Member
Pierre Castellani
Join Date: Apr 2011
Location: Paris
Posts: 38
Rep Power: 15 |
Hi Gökha,
I don't if I could help but what kind of error did you get? Pierre. |
|
March 13, 2012, 10:40 |
|
#3 |
New Member
Join Date: Oct 2011
Posts: 20
Rep Power: 15 |
Hi Pierre,
I played with the relaxation factors and now I am able to run the simulation but results are not like what I expected. Thats why I changed boundaries again like the following lines; for the velocity -- used fixedValue at the inlet, zeroGradient at the outlet. for the pressure -- used zeroGradient at inlet, total pressure at the outlet. With lower relaxation values. It works fine and convergence is fast. But I have a small doubt regarding rho. It seems to be constant. Now trying to understand rho file. |
|
March 15, 2012, 03:28 |
|
#4 |
New Member
Join Date: Apr 2010
Posts: 13
Rep Power: 16 |
Hi,
check the 0/fvsolution file. There is the possibility to enter a rhoMin and rhoMax value. Have you set them to a realistic value for your case? SIMPLE { nNonOrthogonalCorrectors 0; rhoMin rhoMin [1 -3 0 0 0] 0.8; rhoMax rhoMax [1 -3 0 0 0] 1.4; transonic yes; |
|
March 15, 2012, 12:10 |
|
#5 |
New Member
Join Date: Oct 2011
Posts: 20
Rep Power: 15 |
Hi samsi,
you solved my problem. Somehow, I used values 0.1 and 1 which are out of my density range. Now I changed the interval and I am able to see that rho is not constant anymore. Thanks! |
|
April 4, 2012, 05:13 |
|
#6 |
New Member
wangwei
Join Date: Apr 2012
Posts: 9
Rep Power: 14 |
Hi samsi,
can you explain the "transonic yes"? Thank you |
|
April 4, 2012, 08:07 |
|
#7 |
New Member
Join Date: Apr 2010
Posts: 13
Rep Power: 16 |
Hello,
sorry i can't give you an explanation for this... maybe someone else can do this... ? |
|
May 15, 2012, 11:51 |
|
#8 |
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Bad Wörishofen
Posts: 2,711
Blog Entries: 6
Rep Power: 52 |
Hi,
i am not sure if its actuall but the transonic option is a switch in the equation of the pEqn.H file: if transonic true; Code:
{ surfaceScalarField phid ( "phid", fvc::interpolate(psi*U) & mesh.Sf() ); surfaceScalarField phic ( "phic", fvc::interpolate(rho/AtU - rho/AU)*fvc::snGrad(p)*mesh.magSf() + phid*(fvc::interpolate(p) - fvc::interpolate(p, "UD")) ); //refCast<mixedFvPatchScalarField>(p.boundaryField()[1]).refValue() // = p.boundaryField()[1]; fvScalarMatrix pEqn ( fvm::div(phid, p) + fvc::div(phic) - fvm::Sp(fvc::div(phid), p) + fvc::div(phid)*p - fvm::laplacian(rho/AtU, p) ); //pEqn.relax(); pEqn.setReference(pRefCell, pRefValue); pEqn.solve(); if (simple.finalNonOrthogonalIter()) { phi == phic + pEqn.flux(); } } Code:
phi = fvc::interpolate(rho*U) & mesh.Sf(); closedVolume = adjustPhi(phi, U, p); phi += fvc::interpolate(rho/AtU - rho/AU)*fvc::snGrad(p)*mesh.magSf(); fvScalarMatrix pEqn ( fvc::div(phi) //- fvm::laplacian(rho/AU, p) - fvm::laplacian(rho/AtU, p) ); pEqn.setReference(pRefCell, pRefValue); pEqn.solve(); if (simple.finalNonOrthogonalIter()) { phi += pEqn.flux(); } Code:
if (!simple.transonic()) { rho.relax(); } |
|
August 28, 2013, 08:47 |
regarding BC's of rhoSimplecFoam
|
#9 |
Member
sonu
Join Date: Jul 2013
Location: delhi
Posts: 92
Rep Power: 13 |
helo ,
i am trying to simulate cold flow in my case using rhoSimplecFoam . my case is having 2 inlets , upper wall (fixed ), outlet and axis of symmetry . after running the case following error and as per my knowledge it is due to the BC's . So can anybody plz have a look on my BC's and tell me whr i am doin wrong . thanks in advance Code:
Time = 44 GAMG: Solving for Ux, Initial residual = 0.72868, Final residual = 0.0331103, No Iterations 1 GAMG: Solving for Uy, Initial residual = 0.964565, Final residual = 0.00777282, No Iterations 1 GAMG: Solving for e, Initial residual = 0.827116, Final residual = 0.00785967, No Iterations 1 GAMG: Solving for p, Initial residual = 0.242665, Final residual = 0.0241799, No Iterations 2 time step continuity errors : sum local = 0.308447, global = -0.151188, cumulative = -1.05624 rho max/min : 1 0.1 GAMG: Solving for epsilon, Initial residual = 0.089338, Final residual = 1.19406e-05, No Iterations 1 GAMG: Solving for k, Initial residual = 0.778841, Final residual = 0.00695333, No Iterations 1 bounding k, min: 6.9946e-16 max: 2794 average: 2.36892 ExecutionTime = 1150.91 s ClockTime = 1151 s Time = 45 GAMG: Solving for Ux, Initial residual = 0.561691, Final residual = 0.0130153, No Iterations 1 GAMG: Solving for Uy, Initial residual = 0.975585, Final residual = 0.0459448, No Iterations 1 GAMG: Solving for e, Initial residual = 0.908425, Final residual = 0.00318615, No Iterations 2 #0 Foam::error::printStack(Foam::Ostream&) at ??:? #1 Foam::sigFpe::sigHandler(int) at ??:? #2 in "/lib/x86_64-linux-gnu/libc.so.6" #3 Foam::hePsiThermo<Foam::psiThermo, Foam::pureMixture<Foam::sutherlandTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleInternalEnergy> > > >::calculate() at ??:? #4 Foam::hePsiThermo<Foam::psiThermo, Foam::pureMixture<Foam::sutherlandTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleInternalEnergy> > > >::correct() at ??:? #5 at ??:? #6 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6" #7 at ??:? Floating point exception (core dumped) Last edited by wyldckat; August 31, 2013 at 15:52. |
|
Tags |
bcs, boundary conditions, rhosimplecfoam, turbulence, turbulent flows |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Impinging Jet Boundary Conditions | Anindya | Main CFD Forum | 25 | February 27, 2016 13:58 |
symmetry boundary conditions in cfx | lost.identity | CFX | 41 | May 22, 2013 08:21 |
OpenFOAM Variable Velocity Boundary Conditions | NickolasPl | OpenFOAM Programming & Development | 2 | May 19, 2011 06:37 |
[Netgen] boundary conditions and mesh exporting | vaina74 | OpenFOAM Meshing & Mesh Conversion | 2 | May 27, 2010 10:38 |
[Commercial meshers] Trimmed cell and embedded refinement mesh conversion issues | michele | OpenFOAM Meshing & Mesh Conversion | 2 | July 15, 2005 05:15 |