
[Sponsors] 
Periodic flow using Cyclic  comparison with Fluent 

LinkBack  Thread Tools  Search this Thread  Display Modes 
October 19, 2015, 07:41 
Periodic flow using Cyclic  comparison with Fluent

#1 
Member
1214
Join Date: Sep 2015
Posts: 30
Rep Power: 7 
Hello all,
I am fairly new with OpenFOAM and as my first study I am trying to compare OpenFOAM results to the ones obtained to FLUENT. Software versions: OpenFOAM: 2.4.0, FLUENT: 16.1.1 The case I am attempting is a sinusoidal channel  the one which is commonly used in heat exchangers. To eliminate the entrance effects  the flow should be modelled as periodic. The case I ran was at Re=100. Within fluent I set up a Inlet/Outlet as interfaces and connected them using periodic boundary conditions. In terms of periodic conditions I set them us as default in Fluent  as mass flow rate. fluent_velocity.png fluent_pressure.png As of OpenFOAM I imported the fluent mesh, created cyclic boundary conditions and used the fvOptions file to set the momentum source terms using mean velocity to make the things flow. The result I got this was: Openfoam_velocity.png Openfoam_pressure.png As you can see there is a clear difference between the cases. Would anyone have any suggestions why it is happening? Do you have any solutions how to solve this issue? is there a way to put the mass flow rate as a source term to make the correlation easier? The case files are below(The file was too big, thus, had to stick it in dropbox): https://www.dropbox.com/s/8cfncge72e...yclic.zip?dl=0 Thanks for your help in advance! Documentation on such flows is not the best. The code for calculating both mass flow and velocity from Re (matlab): clear clc format long W=2.23e3; % Width of the channel/fin, m H=1; % Height of the channel/fin, m for fluent it is 1 metre for 2D cases L=50e3; % Lenght of the channel/fin, m rho = 1.225; % Density, kg/m^3 mu=1.7894e5; % Dyncamic Viscosity kg/ms nu=mu/rho; % Kinematic viscosity Re=100; % Reynolds number as usual in the papers U_calc=(Re*nu)/(2*W) % If input is velocity they make dh=2W m_dot=rho*U_calc*W*H % Mass flow 

October 19, 2015, 08:45 

#2 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 23 
For iteration 3000 the yplus for the wall is
Patch 1 named WALL y+ : min: 0.28997018732504709071 max: 0.43480356182426332934 average: 0.34463384097139043716 So it is a lowRe mesh. Your boundary conditions are for a highRe mesh. This might explain the difference in velocity plots. Pressure of the incompressible solver is real pressure / density. So you need to multiply the openFoam pressure values by your operating density to compare it to fluent.
__________________
The skeleton ran out of shampoo in the shower. 

October 19, 2015, 10:04 

#3 
Member
1214
Join Date: Sep 2015
Posts: 30
Rep Power: 7 
Hi,
Thanks for reply. I was thinking for a while what you meant by that sentence.. Because I had kEpsilon set as a RAS model with turbulence switched off. Then I actually tried sticking in the laminar RAS model and it made the whole lot of difference. I was mildly surprised by that because I though that when I turned the turbulence off the solver came back to laminar equations, but apparently it did not. The result is: openfoam_vel_fixed.png Openfoam_p_fixed.png As you can see the results are fairly identical  the small differences are cause by discretisation schemes, which are a bit lower accuracy currently set on OpenFOAM. I tried doing that for fluent and it gave me identical result. Thanks for giving me a clue with the pressure! helped a lot. 

October 19, 2015, 10:09 

#4 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 23 
I didn't even recognize that you had turbulence switched off by that setting. I never used that. But anyway now it works
Normally what you did should work. I don't understand why it wasn't switched off.
__________________
The skeleton ran out of shampoo in the shower. 

October 19, 2015, 10:11 

#5 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 23 
Well, maybe with your setting it just doesn't solve for k and epsilon / omega equation but uses the given (\0 directory)entries as fixed settings to calculate the turbulent viscosity...
Edit: I guess this is true. If you set internal k to zero in your \0 directory and restart you will get the correct result.
__________________
The skeleton ran out of shampoo in the shower. 

October 19, 2015, 14:11 

#6 
Member
1214
Join Date: Sep 2015
Posts: 30
Rep Power: 7 
Thanks a lot for your explanation!
In terms of the laminar solver, I managed to get to around Re=400(u=1.310075958634575) where it decided not to converge anymore. Do you have any ideas how to make it more robust? Fluent managed to cope it by using coupled instead of simple. 

October 20, 2015, 02:18 

#7 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 23 
Hi, what do you mean by "more robust"?
__________________
The skeleton ran out of shampoo in the shower. 

October 20, 2015, 10:24 

#8 
Member
1214
Join Date: Sep 2015
Posts: 30
Rep Power: 7 
Hi,
by that I meant make it to work for broader range of Re. When I increased Re number for the case to Re = 400 (Ubar ~ 1.31). It caused fluctuations in the solution, whilst the FLUENT with coupled algorithm managed to converge. Do you know any tips how to avoid it? 

October 20, 2015, 10:34 

#9 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 23 
"fluctuations" in the residuals or where?
__________________
The skeleton ran out of shampoo in the shower. 

October 20, 2015, 10:43 

#10 
Member
1214
Join Date: Sep 2015
Posts: 30
Rep Power: 7 
Hi,
I will explain it better. The residuals: Re400laminar.png Screenshots of contours every thousand of iterations: 8000: RE_400_iter_8000.png 9000: RE_400_iter_9000.png 10000: RE_400_iter_10000.png 

October 20, 2015, 10:44 

#11 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 23 
Well that doesn't converge.
Can you post your fvSolution, fvSchemes and the last iterations of the log file?
__________________
The skeleton ran out of shampoo in the shower. 

October 20, 2015, 10:51 

#12 
Member
1214
Join Date: Sep 2015
Posts: 30
Rep Power: 7 
Sure, hopefully it does not too messy for you:
end of the log: Code:
Time = 9295 smoothSolver: Solving for Ux, Initial residual = 0.0030142261772487153292, Final residual = 0.00018070334041139326825, No Iterations 2 smoothSolver: Solving for Uy, Initial residual = 0.0053867800424603354617, Final residual = 0.00033189147557002824729, No Iterations 2 Pressure gradient source: uncorrected Ubar = 1.3100603632674117094, pressure gradient = 545.82799332159220285 GAMG: Solving for p, Initial residual = 0.06511037145398994308, Final residual = 0.0041452058269561622983, No Iterations 2 time step continuity errors : sum local = 0.51530691506081338638, global = 9.6585870312325598997e06, cumulative = 0.089760748431006662229 Pressure gradient source: uncorrected Ubar = 1.3100815117520456798, pressure gradient = 542.91507642249086985 ExecutionTime = 120.35999999999999943 s ClockTime = 120 s Time = 9296 smoothSolver: Solving for Ux, Initial residual = 0.0029965368759614871043, Final residual = 0.0001785926573439436415, No Iterations 2 smoothSolver: Solving for Uy, Initial residual = 0.0054422825121599408688, Final residual = 0.00033430076309385209918, No Iterations 2 Pressure gradient source: uncorrected Ubar = 1.3100597716058490771, pressure gradient = 545.14540749593311375 GAMG: Solving for p, Initial residual = 0.06451587043113798936, Final residual = 0.003530805916910612248, No Iterations 2 time step continuity errors : sum local = 0.4415437208139421088, global = 9.6587834832260265847e06, cumulative = 0.089770407214489894576 Pressure gradient source: uncorrected Ubar = 1.3100822717510278714, pressure gradient = 542.04522315703286495 ExecutionTime = 120.37999999999999545 s ClockTime = 120 s Time = 9297 smoothSolver: Solving for Ux, Initial residual = 0.003021439132626162552, Final residual = 0.00017980854255233262042, No Iterations 2 smoothSolver: Solving for Uy, Initial residual = 0.0053910275692351083271, Final residual = 0.00033061411398559788655, No Iterations 2 Pressure gradient source: uncorrected Ubar = 1.3100620085433221096, pressure gradient = 543.96790143860755506 GAMG: Solving for p, Initial residual = 0.06527820975546982929, Final residual = 0.0042271249612424203687, No Iterations 2 time step continuity errors : sum local = 0.55618282819879694134, global = 9.6590992031169466126e06, cumulative = 0.089780066313693007718 Pressure gradient source: uncorrected Ubar = 1.3100792798772626924, pressure gradient = 541.58747122782585848 ExecutionTime = 120.39000000000000057 s ClockTime = 120 s Time = 9298 smoothSolver: Solving for Ux, Initial residual = 0.0029947009240669690902, Final residual = 0.00017771144110895249909, No Iterations 2 smoothSolver: Solving for Uy, Initial residual = 0.0054590914567207446742, Final residual = 0.00033386662296646844135, No Iterations 2 Pressure gradient source: uncorrected Ubar = 1.3100607748466328584, pressure gradient = 543.68067534449471623 GAMG: Solving for p, Initial residual = 0.063088913975031510328, Final residual = 0.0039161000397144908602, No Iterations 2 time step continuity errors : sum local = 0.48745883414103380327, global = 9.6591822411424853908e06, cumulative = 0.089789725495934155641 Pressure gradient source: uncorrected Ubar = 1.3100830731378683147, pressure gradient = 540.60668121425521804 ExecutionTime = 120.40000000000000568 s ClockTime = 120 s Time = 9299 smoothSolver: Solving for Ux, Initial residual = 0.0030144707107860281223, Final residual = 0.00017813898387061542533, No Iterations 2 smoothSolver: Solving for Uy, Initial residual = 0.0054223025449059549311, Final residual = 0.00033097957930049420189, No Iterations 2 Pressure gradient source: uncorrected Ubar = 1.3100626629309388704, pressure gradient = 542.4399464015061767 GAMG: Solving for p, Initial residual = 0.064360624329235463503, Final residual = 0.003574292542555871071, No Iterations 2 time step continuity errors : sum local = 0.47073056129697354866, global = 9.6593609382747772503e06, cumulative = 0.089799384856872430105 Pressure gradient source: uncorrected Ubar = 1.3100810319135225424, pressure gradient = 539.90715707213769292 ExecutionTime = 120.42000000000000171 s ClockTime = 120 s Time = 9300 smoothSolver: Solving for Ux, Initial residual = 0.0030060085023729749346, Final residual = 0.0001775962916378959059, No Iterations 2 smoothSolver: Solving for Uy, Initial residual = 0.0054377854809080318141, Final residual = 0.00033143736345043990155, No Iterations 2 Pressure gradient source: uncorrected Ubar = 1.3100633286004443878, pressure gradient = 541.64885297837497546 GAMG: Solving for p, Initial residual = 0.062612587898651206331, Final residual = 0.0040836100267523317911, No Iterations 2 time step continuity errors : sum local = 0.50924408601294590682, global = 9.659438363008983355e06, cumulative = 0.08980904429523543786 Pressure gradient source: uncorrected Ubar = 1.3100836275253004981, pressure gradient = 538.84960841913800778 ExecutionTime = 120.43000000000000682 s ClockTime = 120 s Time = 9301 smoothSolver: Solving for Ux, Initial residual = 0.0029993729454928868237, Final residual = 0.00017639142097321101497, No Iterations 2 smoothSolver: Solving for Uy, Initial residual = 0.0054679932764793289998, Final residual = 0.00033218215220257886738, No Iterations 2 Pressure gradient source: uncorrected Ubar = 1.3100633575023452604, pressure gradient = 540.58746802936445874 GAMG: Solving for p, Initial residual = 0.062273976018851491532, Final residual = 0.0030614791476954047143, No Iterations 2 time step continuity errors : sum local = 0.40569798671617252062, global = 9.6595026991233798341e06, cumulative = 0.08981870379793456538 Pressure gradient source: uncorrected Ubar = 1.3100788330487438405, pressure gradient = 538.45318941518178235 ExecutionTime = 120.45000000000000284 s ClockTime = 120 s Time = 9302 smoothSolver: Solving for Ux, Initial residual = 0.0030126219283441268808, Final residual = 0.00017685873923883887755, No Iterations 2 smoothSolver: Solving for Uy, Initial residual = 0.0054212643616981508882, Final residual = 0.0003293912110210666733, No Iterations 2 Pressure gradient source: uncorrected Ubar = 1.3100658910909372956, pressure gradient = 539.84167044233481647 GAMG: Solving for p, Initial residual = 0.062754410783897957016, Final residual = 0.0041134422295080593987, No Iterations 2 time step continuity errors : sum local = 0.51270005829692355537, global = 9.6596181861437968927e06, cumulative = 0.089828363416120715623 Pressure gradient source: uncorrected Ubar = 1.3100831747255314852, pressure gradient = 537.45797094441934405 ExecutionTime = 120.45999999999999375 s ClockTime = 120 s Time = 9303 smoothSolver: Solving for Ux, Initial residual = 0.002990507618087509447, Final residual = 0.00017533903922666086968, No Iterations 2 smoothSolver: Solving for Uy, Initial residual = 0.0054850112576477674103, Final residual = 0.00033195624508595321855, No Iterations 2 Pressure gradient source: uncorrected Ubar = 1.3100648542525064055, pressure gradient = 538.98941952984546333 GAMG: Solving for p, Initial residual = 0.061633026457751864668, Final residual = 0.0029219085350524580391, No Iterations 2 time step continuity errors : sum local = 0.38715982644265090062, global = 9.6595322213938960524e06, cumulative = 0.08983802294834210278 Pressure gradient source: uncorrected Ubar = 1.3100749450238227123, pressure gradient = 537.59776195152642231 ExecutionTime = 120.46999999999999886 s ClockTime = 120 s fvSchemes: Code:
/** C++ **\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 2.4.0   \\ / 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; grad(U) cellLimited Gauss linear 1; } divSchemes { default none; div(phi,U) bounded Gauss upwind; // div(phi,k) bounded Gauss upwind; // div(phi,epsilon) bounded Gauss upwind; div(phi,R) bounded Gauss upwind; div(R) Gauss linear; // div(phi,nuTilda) bounded Gauss upwind; div((nuEff*dev(T(grad(U))))) Gauss linear; } laplacianSchemes { default Gauss linear corrected; } interpolationSchemes { default linear; } fluxRequired { default no; p; Phi; } // ************************************************************************* // fvSolution: Code:
/** C++ **\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 2.4.0   \\ / A nd  Web: www.OpenFOAM.org   \\/ M anipulation   \**/ FoamFile { version 2.0; format ascii; class dictionary; location "system"; object fvSolution; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // solvers { Phi { $p; } potentialFlow { nNonOrthogonalCorrectors 10; } cache { grad(U); } p { solver GAMG; tolerance 1e20; relTol 0.1; smoother GaussSeidel; nPreSweeps 0; nPostSweeps 2; cacheAgglomeration on; agglomerator faceAreaPair; nCellsInCoarsestLevel 10; mergeLevels 1; } "(UkepsilonRnuTilda)" { solver smoothSolver; smoother symGaussSeidel; tolerance 1e20; relTol 0.1; } } SIMPLE { nNonOrthogonalCorrectors 0; pRefCell 1001; pRefValue 0; residualControl { p 1e20; U 1e20; "(kepsilonomega)" 1e20; } } relaxationFactors { fields { p 0.5; } equations { U 0.7; k 0.7; epsilon 0.7; R 0.7; nuTilda 0.7; } } // ************************************************************************* // 

October 20, 2015, 10:59 

#13 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 23 
For me it looks like you already have pretty safe settings.
You are using cyclic boundary conditions? I tryed to get them running for different very similar cases, namely a straight pipe and a channel flow. Both of them did not converge properly no matter what numerical settings I used. I eventually used the "mapped" boundary condition instead of the cyclic, which does pretty much the same for this kind of set up. That worked without any problems. I suspect that there is some issue with the solver and cyclic b.c.  or I am simply incompetent, which could be taken into account.
__________________
The skeleton ran out of shampoo in the shower. 

October 20, 2015, 11:04 

#14 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 23 
Here is the thread:
http://www.cfdonline.com/Forums/ope...tml#post521820
__________________
The skeleton ran out of shampoo in the shower. 

October 20, 2015, 11:27 

#15 
Member
1214
Join Date: Sep 2015
Posts: 30
Rep Power: 7 
Ok, I will attempt to modify everything into the mapped conditions and I will post the results.
I did try using the mapped condiitons initially without too much luck,but again, my knowledge of OpenFOAM increases significantly every day. 

October 20, 2015, 13:30 

#16 
Member
1214
Join Date: Sep 2015
Posts: 30
Rep Power: 7 
Ok.. So I did try it and I think cyclic is better than mapped in my case at least when everything is periodic.. I will explain why and give the bits and pieces of code.
So, for mapped case. I used Re=200 case which works well everywhere. Boundary file: Code:
/** C++ **\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 2.4.0   \\ / A nd  Web: www.OpenFOAM.org   \\/ M anipulation   \**/ FoamFile { version 2.0; format ascii; class polyBoundaryMesh; location "constant/polyMesh"; object boundary; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // 4 ( OUTLET { type patch; nFaces 59; startFace 21937; } WALL { type wall; inGroups 1(wall); nFaces 376; startFace 21996; } INLET { type mappedPatch; inGroups 1(mappedPatch); nFaces 59; startFace 22372; sampleMode nearestPatchFace;//nearestCell; sampleRegion region0; samplePatch OUTLET; offsetMode uniform; offset (0.00628 0 0); //type patch; //nFaces 59; //startFace 22372; } frontAndBackPlanes { type empty; inGroups 1(empty); nFaces 22184; startFace 22431; } ) // ************************************************************************* // Code:
/** C++ **\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 2.4.0   \\ / A nd  Web: www.OpenFOAM.org   \\/ M anipulation   \**/ FoamFile { version 2.0; format ascii; class volVectorField; location "0"; object U; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 1 1 0 0 0 0]; internalField uniform (0.655037979317287 0 0); boundaryField { INLET { type mapped; value uniform (0.655037979317287 0 0); interpolationScheme cell; setAverage true; average (0.655037979317287 0 0); //type fixedValue; //value uniform (1.31 0 0); } OUTLET { type fixedValue; value $internalField; } WALL { type fixedValue; value uniform (0 0 0); } frontAndBackPlanes { type empty; } } // ************************************************************************* // Code:
/** C++ **\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 2.4.0   \\ / A nd  Web: www.OpenFOAM.org   \\/ M anipulation   \**/ FoamFile { version 2.0; format ascii; class volScalarField; object p; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 2 2 0 0 0 0]; internalField uniform 0; boundaryField { INLET { type mapped; value $internalField; interpolationScheme cell; setAverage true; average 0; //type fixedValue; //value $internalField; } OUTLET { type fixedValue; value $internalField; } WALL { type zeroGradient; } frontAndBackPlanes { type empty; } } // ************************************************************************* // And it gives a result: RE200_residuals.png RE200_vel.png RE_200_p.png Applying cyclic condition as before, meanwhile, gives: RE_200_vel_cyclic.png RE_200_p_cyclic.png Using FLUENT is on another message as I ran out of maximum attachment number. 

October 20, 2015, 13:35 

#17 
Member
1214
Join Date: Sep 2015
Posts: 30
Rep Power: 7 
So, using Fluent gives:
RE_200_u_fluent.png RE_200_p_fluent.png As you can see fluent agrees fairly well with the cyclic condition and for mapped condition.. not so much. There are some settings as you may know as well whilst using the mapped boundary condition complicated to make it truly cyclic. As of Re = 400 both fluent and OpenFOAM struggle.. So, I have tried several turbulence models as well to see what is happening. I know RE number is low, but again, the geometry of the problem is such that flow would be disturbed to maximum. So, I have got some Results which are in the following messages. 

October 20, 2015, 13:47 

#18 
Member
1214
Join Date: Sep 2015
Posts: 30
Rep Power: 7 
So, using now FLUENT with COUPLED (Simple misbehaved and did not converge s in OpenFOAM) to predict flow at Re=400 and laminar:
fluent_laminar_u.png fluent_lam_p.png Openfoam on laminar: open_lam_u.png open_lam_p.png 

October 20, 2015, 13:49 

#19 
Member
1214
Join Date: Sep 2015
Posts: 30
Rep Power: 7 
So, the next step was to use kepsilon (because why not). Again, FLUENT:
fluent_keu.png fluent_ke_p.png Openfoam open_keu.png open_kep.png Residuals: openkeres.png Looks like a fair match between the two 

October 20, 2015, 13:54 

#20 
Member
1214
Join Date: Sep 2015
Posts: 30
Rep Power: 7 
And finally komegaSST (because why not again). Fluent:
fluent_kou.png fluentkop.png OpenFOAM: open_kou.png openkop.png and residuals: kores.png Again, not horrific match, however, as can be seen the result did not converge that well. I have noticed this before, that somehow the kOmegaSST is much more sensitive to the initial conditions (my guess) which consequently causes all of this. It did work reasonably for the simple inlet/outlet case, suggesting that cyclic conditions might cause that as well to some extent. To avoid this, I was planing to make a quick code to estimate everything. Unless your opinion of this is different. Or maybe you know the app for estimating quantities within OpenFOAM already exists? 

Tags 
fluent, openfoam, periodic flow 
Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Periodic Pipe Flow LES  dvolkind  CFX  8  March 21, 2020 06:30 
No flow through periodic (cyclic) boundaries in impeller with foamextend3.1  anttiad9000  OpenFOAM Running, Solving & CFD  3  March 2, 2016 20:37 
Fluent v15 multiphase flow b.c. failure Nonchannel flow  mickjazz  Fluent Multiphase  1  September 22, 2014 07:41 
Comparison between Solidworks Flow Simulation and Ansys Fluent  Bruce828  Main CFD Forum  5  February 23, 2013 11:13 
Split boundary zone in FLUENT for mass flow  eishinsnsayshin  FLUENT  1  January 18, 2013 14:43 