
[Sponsors] 
March 14, 2017, 13:06 
Proper settings for PimpleFoam Simulation

#1 
New Member
Join Date: Oct 2016
Posts: 22
Rep Power: 6 
Hello,
I want to do a 3D transient simulation of a wing. However, I am not able to get pimple to converge. Maybe somebody can give me a hint. so heres what I do: I start the simulation with SimpleFoam and calculate 5000 timesteps. After that I switch to Pimple. My Settings are like this: Control dict: Code:
/** C++ **\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 4.1   \\ / A nd  Web: www.OpenFOAM.org   \\/ M anipulation   \**/ FoamFile { version 2.0; format ascii; class dictionary; location "system"; object controlDict; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // application pimpleFoam; startFrom latestTime; startTime 0; stopAt endTime; endTime 5002; deltaT 5e6; writeControl timeStep; writeInterval 10000; purgeWrite 0; writeFormat ascii; writePrecision 7; writeCompression off; timeFormat general; timePrecision 6; runTimeModifiable true; maxCo 2; maxDeltaT 1; functions { #include "forceCoeffs" } // ************************************************************************* // Code:
/** C++ **\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 4.1   \\ / A nd  Web: www.OpenFOAM.org   \\/ M anipulation   \**/ FoamFile { version 2.0; format ascii; class dictionary; location "system"; object fvSolution; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // /*The solver stops if any one of the following conditions are reached: • the residual falls below the solver tolerance, tolerance ; • the ratio of current to initial residuals falls below the solver relative tolerance, relTol; • the number of iterations exceeds a maximum number of iterations, maxIter;*/ solvers { p { solver GAMG; smoother DICGaussSeidel; tolerance 4e4; relTol 0.001; } pFinal { $p; relTol 0; } "(Ukepsilonomega)" { solver smoothSolver; smoother symGaussSeidel; tolerance 1e6; relTol 0.1; } "(Ukepsilonomega)Final" { $U; relTol 0; } } PIMPLE { nNonOrthogonalCorrectors 0; // Korrigieren des Drucks mit den neu berechneten Drücken nOuterCorrectors 70; // Berechnung des Drucks  Momenten Kopplung nCorrectors 2; // korrigieren des Drucks relaxationFactors { fields { p 0.2; pFinal 1; // Last outer loop } equations { U 0.6; UFinal 1;// Last outer loop } } residualControl { p { relTol 0; // If this inital tolerance is reached, leave tolerance 1e3; } U { relTol 0; // If this inital tolerance is reached, leave tolerance 1e4; } } } // ************************************************************************* // Code:
/** C++ **\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 4.1   \\ / A nd  Web: www.OpenFOAM.org   \\/ M anipulation   \**/ FoamFile { version 2.0; format ascii; class dictionary; object fvSchemes; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // ddtSchemes { //default Euler; //transient, first order implicit, bounded. //default backward;//transient, second order implicit, potentially unbounded default CrankNicolson 0.9;//ransient, second order implicit, bounded; requires an offcentering //coefficient } gradSchemes { default Gauss linear; } snGradSchemes { default corrected; //The corrected scheme is generally recommended, //but for maximum nonorthogonality above 70, limited //may be required. //default uncorrected; //default limited corrected 0.33; //Typically,psi is chosen to be 0.33 or //0.5, where 0.33 offers greater stabilit //y and 0.5 greater accuracy. } divSchemes { //Konservativ Wolfgang /*default none; div(phi,U) Gauss upwind; div(phi,k) Gauss upwind; div(phi,epsilon) Gauss upwind; div(phi,omega) Gauss limitedLinear 1; div(phi,R) Gauss upwind; div(R) Gauss linear; div(phi,nuTilda) Gauss upwind; div((nuEff*dev2(T(grad(U))))) Gauss linear; */ //Aggressiv Wolfgang /*default none; div(phi,U) Gauss limitedLinearV 1; div(phi,k) Gauss limitedLinearV 1; div(phi,epsilon) Gauss limitedLinearV 1; div(phi,omega) Gauss limitedLinearV 1; div(phi,R) Gauss linear; div(R) Gauss linear; div(phi,nuTilda) Gauss linear; div((nuEff*dev2(T(grad(U))))) Gauss linear; */ //Tutorials default none; div(phi,U) bounded Gauss linearUpwind grad(U); div(phi,k) bounded Gauss upwind; div(phi,epsilon) bounded Gauss upwind; div(phi,omega) bounded Gauss upwind; div(phi,R) bounded Gauss upwind; div(R) Gauss linear; div(phi,nuTilda) bounded Gauss upwind; div((nuEff*dev2(T(grad(U))))) Gauss linear; } laplacianSchemes { default Gauss linear corrected; laplacian(rAUf,p) Gauss linear corrected; } interpolationSchemes { default linear; } wallDist { method meshWave; } // ************************************************************************* // Code:
Create time Create mesh for time = 5000 PIMPLE: max iterations = 70 field p : relTol 0, tolerance 0.001 field U : relTol 0, tolerance 0.0001 Reading field p Reading field U Reading/calculating face flux field phi Selecting incompressible transport model Newtonian Selecting turbulence model type RAS Selecting RAS turbulence model kOmegaSST Selecting patchDistMethod meshWave kOmegaSSTCoeffs { alphaK1 0.85; alphaK2 1; alphaOmega1 0.5; alphaOmega2 0.856; gamma1 0.5555556; gamma2 0.44; beta1 0.075; beta2 0.0828; betaStar 0.09; a1 0.31; b1 1; c1 10; F3 false; } No MRF models present No finite volume options present Starting time loop forces forces: Not including porosity effects Courant Number mean: 0.0009207056 max: 5.870972 Time = 5000 PIMPLE: iteration 1 smoothSolver: Solving for Ux, Initial residual = 1.755553e07, Final residual = 1.755553e07, No Iterations 0 smoothSolver: Solving for Uy, Initial residual = 6.909956e10, Final residual = 6.909956e10, No Iterations 0 smoothSolver: Solving for Uz, Initial residual = 1.712918e09, Final residual = 1.712918e09, No Iterations 0 GAMG: Solving for p, Initial residual = 0.8733274, Final residual = 0.0008564715, No Iterations 51 time step continuity errors : sum local = 9.58361e13, global = 4.116155e15, cumulative = 4.116155e15 GAMG: Solving for p, Initial residual = 0.6793104, Final residual = 0.0006542594, No Iterations 58 time step continuity errors : sum local = 1.029039e12, global = 3.69671e14, cumulative = 3.285095e14 PIMPLE: iteration 2 smoothSolver: Solving for Ux, Initial residual = 1.232057e06, Final residual = 4.12252e11, No Iterations 1 smoothSolver: Solving for Uy, Initial residual = 3.331185e09, Final residual = 3.331185e09, No Iterations 0 smoothSolver: Solving for Uz, Initial residual = 1.43496e08, Final residual = 1.43496e08, No Iterations 0 GAMG: Solving for p, Initial residual = 0.7188413, Final residual = 0.0006887674, No Iterations 60 time step continuity errors : sum local = 9.293172e13, global = 6.52682e15, cumulative = 3.937777e14 GAMG: Solving for p, Initial residual = 0.6790615, Final residual = 0.0006542149, No Iterations 58 time step continuity errors : sum local = 1.028279e12, global = 3.61447e14, cumulative = 7.552246e14 PIMPLE: iteration 3 smoothSolver: Solving for Ux, Initial residual = 1.196535e06, Final residual = 3.577596e11, No Iterations 1 smoothSolver: Solving for Uy, Initial residual = 3.238559e09, Final residual = 3.238559e09, No Iterations 0 smoothSolver: Solving for Uz, Initial residual = 1.399866e08, Final residual = 1.399866e08, No Iterations 0 GAMG: Solving for p, Initial residual = 0.7186701, Final residual = 0.0006886802, No Iterations 60 time step continuity errors : sum local = 9.291727e13, global = 6.536857e15, cumulative = 8.205932e14 GAMG: Solving for p, Initial residual = 0.6790486, Final residual = 0.0006542245, No Iterations 58 time step continuity errors : sum local = 1.028292e12, global = 3.614505e14, cumulative = 1.182044e13 PIMPLE: iteration 4 smoothSolver: Solving for Ux, Initial residual = 1.196485e06, Final residual = 3.539771e11, No Iterations 1 smoothSolver: Solving for Uy, Initial residual = 3.238436e09, Final residual = 3.238436e09, No Iterations 0 smoothSolver: Solving for Uz, Initial residual = 1.399785e08, Final residual = 1.399785e08, No Iterations 0 GAMG: Solving for p, Initial residual = 0.718663, Final residual = 0.0006886793, No Iterations 60 time step continuity errors : sum local = 9.291714e13, global = 6.536782e15, cumulative = 1.247412e13 GAMG: Solving for p, Initial residual = 0.6790474, Final residual = 0.0006542243, No Iterations 58 time step continuity errors : sum local = 1.028292e12, global = 3.614506e14, cumulative = 1.608862e13 PIMPLE: iteration 5 smoothSolver: Solving for Ux, Initial residual = 1.19648e06, Final residual = 3.533432e11, No Iterations 1 smoothSolver: Solving for Uy, Initial residual = 3.238428e09, Final residual = 3.238428e09, No Iterations 0 smoothSolver: Solving for Uz, Initial residual = 1.399783e08, Final residual = 1.399783e08, No Iterations 0 GAMG: Solving for p, Initial residual = 0.7186625, Final residual = 0.0006886793, No Iterations 60 time step continuity errors : sum local = 9.291714e13, global = 6.536782e15, cumulative = 1.67423e13 GAMG: Solving for p, Initial residual = 0.6790473, Final residual = 0.0006542243, No Iterations 58 time step continuity errors : sum local = 1.028292e12, global = 3.614506e14, cumulative = 2.035681e13 PIMPLE: iteration 6 smoothSolver: Solving for Ux, Initial residual = 1.196477e06, Final residual = 3.531863e11, No Iterations 1 smoothSolver: Solving for Uy, Initial residual = 3.238427e09, Final residual = 3.238427e09, No Iterations 0 smoothSolver: Solving for Uz, Initial residual = 1.399782e08, Final residual = 1.399782e08, No Iterations 0 GAMG: Solving for p, Initial residual = 0.7186624, Final residual = 0.0006886793, No Iterations 60 time step continuity errors : sum local = 9.291714e13, global = 6.536782e15, cumulative = 2.101048e13 GAMG: Solving for p, Initial residual = 0.6790472, Final residual = 0.0006542243, No Iterations 58 time step continuity errors : sum local = 1.028292e12, global = 3.614506e14, cumulative = 2.462499e13 PIMPLE: iteration 7 smoothSolver: Solving for Ux, Initial residual = 1.196477e06, Final residual = 3.531392e11, No Iterations 1 smoothSolver: Solving for Uy, Initial residual = 3.238427e09, Final residual = 3.238427e09, No Iterations 0 smoothSolver: Solving for Uz, Initial residual = 1.399782e08, Final residual = 1.399782e08, No Iterations 0 GAMG: Solving for p, Initial residual = 0.7186624, Final residual = 0.0006886793, No Iterations 60 time step continuity errors : sum local = 9.291714e13, global = 6.536782e15, cumulative = 2.527867e13 GAMG: Solving for p, Initial residual = 0.6790472, Final residual = 0.0006542243, No Iterations 58 time step continuity errors : sum local = 1.028292e12, global = 3.614506e14, cumulative = 2.889318e13 PIMPLE: iteration 8 smoothSolver: Solving for Ux, Initial residual = 1.196477e06, Final residual = 3.531239e11, No Iterations 1 smoothSolver: Solving for Uy, Initial residual = 3.238426e09, Final residual = 3.238426e09, No Iterations 0 smoothSolver: Solving for Uz, Initial residual = 1.399782e08, Final residual = 1.399782e08, No Iterations 0 GAMG: Solving for p, Initial residual = 0.7186624, Final residual = 0.0006886793, No Iterations 60 time step continuity errors : sum local = 9.291714e13, global = 6.536782e15, cumulative = 2.954685e13 GAMG: Solving for p, Initial residual = 0.6790472, Final residual = 0.0006542243, No Iterations 58 time step continuity errors : sum local = 1.028292e12, global = 3.614506e14, cumulative = 3.316136e13 Hope somebody can help me? Thanks a lot in advance!! 

March 15, 2017, 09:44 

#2 
Senior Member

Hi,
I would think you should try this (might even use 0.9 if it is stable): Code:
relaxationFactors { fields { p 0.8; pFinal 1; // Last outer loop } equations { U 0.8; UFinal 1;// Last outer loop } 

March 15, 2017, 10:07 

#3 
New Member
Join Date: Oct 2016
Posts: 22
Rep Power: 6 
Hey Tom,
thanks for your reply. I will definitely try to increase the relaxation factors. However I thought making the relaxation factors bigger will make it more difficult for Pimple to converge. Thus i started with small relaxation factors. Am I wrong with this? Best, Mahe 

March 15, 2017, 10:22 

#4 
Senior Member

Hi Mahe,
Well for p you are relaxing the field, so it can only change by URF*(pp_old), which means that changes in the field are slow with low underrelaxation. It may be that with too high URF your system becomes unstable and therefore cannot converge anymore. My experience with PIMPLE thus far is that 0.80.9 gives usually the best performance, but you will have to play around a bit for each particular case. Regards, Tom 

March 16, 2017, 06:10 

#5 
New Member
Join Date: Oct 2016
Posts: 22
Rep Power: 6 
Hey Tom,
Thanks a lot for your help. It's good to know there is somebody out there helping So to sum it up and get it right: small relaxation factors = slow convergence, but stable high relaxation factors = fast convergence, maybe unstable? I have tried the settings you suggested, but still PIMPLE says it doesn't converge after the 20 iterations I have set. Therefore the simulation is not moving on in time. I am kind of lost now. I do not really care about my pressure residual. I mean it could be 0.1 and still the simulation could get me good results in forces, right? Furthermore I ran the same case in steadystate and the residual didn't change a lot, for the pressure it was around 0.1 to 0.01 and the forces were also stable. So how can I achieve the simulation just starts and moves on and then see how it goes? I took the residual control out and though the simulation will just calculate the timesteps, but it doesn't... thanks! 

March 16, 2017, 06:22 

#6 
Senior Member

Hi Mahe,
I just had a closer look at your output, it looks like the pressure equations need a lot of iterations maybe you can change the relTol for pressure solver to 0.05. If this does not help to get No Iterations down, then I think something is wrong with either mesh or boundary conditions, but than again you did get a result from simpleFoam. I would also suggest to make your pimpleFoam case separate from the simpleFoam case by copying the files from the 5000 folder to a new 0 folder and then run to endTime 2. If you want to keep it like this I would suggest to increase the time precision in controlDict to 12. Regards, Tom 

March 16, 2017, 06:41 

#7 
New Member
Join Date: Oct 2016
Posts: 22
Rep Power: 6 
Hey Tom,
wow. Incredibly fast answer! Thanks for that. Actually I just had the same idea with creating a new folder and just did that an hour ago or so I will try to change relTol. Thanks! Well, I am not to sure about the mesh, since this is my first 3D simulation and I am also not too familiar with OpenFoam and especially SnappyHexMesh. However when I run a checkMesh, it seems to be ok. Code:
/**\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 3.0.1   \\ / A nd  Web: www.OpenFOAM.org   \\/ M anipulation   \**/ Build : 3.0.1119cac7e8750 Exec : checkMesh Date : Mar 16 2017 Time : 11:26:35 Host : PID : 3448 Case : / nProcs : 1 sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). fileModificationChecking : Monitoring runtime modified files using timeStampMaster allowSystemOperations : Allowing usersupplied system call operations // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create polyMesh for time = 0 Time = 0 Mesh stats points: 9513444 faces: 27400550 internal faces: 27074847 cells: 8952175 faces per cell: 6.085158 boundary patches: 6 point zones: 0 face zones: 0 cell zones: 0 Overall number of cells of each type: hexahedra: 8487632 prisms: 43938 wedges: 0 pyramids: 0 tet wedges: 625 tetrahedra: 0 polyhedra: 419980 Breakdown of polyhedra by number of faces: faces number of cells 4 12760 5 12992 6 79719 7 123390 8 33519 9 105541 10 3007 11 970 12 36939 13 93 14 114 15 10765 16 7 17 2 18 162 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 9900 10101 ok (nonclosed singly connected) Outlet 9900 10101 ok (nonclosed singly connected) Innen 51509 52440 ok (nonclosed singly connected) Aussen 19250 19536 ok (nonclosed singly connected) ObenandUnten 31500 32032 ok (nonclosed singly connected) Wing 203644 222844 ok (nonclosed singly connected) Checking geometry... Overall domain bounding box (53.6 30 30) (80 46 30) Mesh has 3 geometric (nonempty/wedge) directions (1 1 1) Mesh has 3 solution (nonempty) directions (1 1 1) Boundary openness (2.550842e14 1.535069e15 6.200779e17) OK. Max cell openness = 5.294373e16 OK. Max aspect ratio = 63.15114 OK. Minimum face area = 8.686202e10. Maximum face area = 7.637955. Face area magnitudes OK. Min volume = 1.025883e12. Max volume = 14.76541. Total volume = 120384. Cell volumes OK. Mesh nonorthogonality Max: 65.07734 average: 5.86854 Nonorthogonality check OK. Face pyramids OK. Max skewness = 3.923949 OK. Coupled point location match (average 0) OK. Mesh OK. End 1. What counts for the pimple loop to end is the last Initial residual, right? 2. In every calculation step, Initial residual is p_old and final residual is p in your equation URF*(pp_old)? => so multiplied with my relaxation factor it should give me the new Initial residual? 3. Still I am not sure, why my initial pressure residual starts with the same value for every iteration?! Shouldn't use the former calculated ones? Sorry for all the questions and again, thanks so much for your help!! My next steps will be: 1 changing the relTol 2 increase nNonOrthogonalCorrectors and see if it is better to recalculate the pressure in every iteration, since there it does decrease. I will let you know how this goes! Best, Mahe 

March 16, 2017, 07:16 

#8 
Senior Member
Oskar
Join Date: Nov 2015
Location: Poland
Posts: 185
Rep Power: 7 
Hello.
Look at those three lines in Your checkMesh: 1. Max aspect ratio = 63... (I think it its pretty high) 2. Mesh nonorthogonality Max = 65 (I think it its pretty high) 3. Min volume = 1.025883e12. Max volume = 14.76541. (Isn't that meshcell too big?) Maybe there is an answer? You should prepare better mesh. Or maybe You should try to set Your PIMPLE nNonOrthogonalCorrectors to something like 2  5. Have a nice day. 

March 16, 2017, 07:29 

#9 
New Member
Join Date: Oct 2016
Posts: 22
Rep Power: 6 
Hey sheaker,
thanks for your answer. As I stated I use OpenFoam for about 5 months and SnappyHexMesh for maybe 2. I need it for my masterthesis. Therefore I am not completely sure what the maximum numbers are and trusted the checkMesh output. Another thing is that you have to specify every parameter of the Mesh, run SHM and then check the result. I am not sure how to find the places, where to increase the Mesh and even when how to fix that particular spot. Also I am a bit limited by my resources. My Mesh now has around 810mio cells which I don't want to increase much. Additionally I am calculating an wing, so I have small cells near the Wingsurface but the cells in the farfield are big (100m away). As I expect there isn't much going on at the farfield and therefore the big cells should be ok?! Best, Mahe 

March 16, 2017, 09:39 

#10 
Senior Member
Uwe Pilz
Join Date: Feb 2017
Location: Leipzig, Germany
Posts: 590
Rep Power: 9 
As I wrote somewhere else, the Courant number is a better measure for the quality of you mesh. It describes the mesh under flow conditions. The relation between maximal and mean Courant number should be small. This evaluation may be done with an imperfect mesh.
__________________
Uwe Pilz  Die der Hauptbewegung überlagerte Schwankungsbewegung ist in ihren Einzelheiten so hoffnungslos kompliziert, daß ihre theoretische Berechnung aussichtslos erscheint. (Hermann Schlichting, 1950) 

March 16, 2017, 10:19 

#11 
Senior Member

Hi Piu,
I do not agree with your statement. It may be related to the efficiency of the mesh (especially for interior domain simulations), but if you use large cells in the outer domain of your mesh and small cells near the surface there is always going to be a large difference between mean and max value of the Courant number. This does not mean you have a bad quality mesh. With regards to the checkMesh report, I would agree that the nonorthogonality and skewness are a bit high. You may want to change these in the settings for quality with snappyHexMesh, but take care that there is still a decent boundary layer mesh. The aspect ratio does not scare me at all. Should be fine in case of boundary layer meshes. In fact I have had much higher aspect ratios and had no problems. Regards, Tom 

March 16, 2017, 11:48 

#12 
Senior Member
Uwe Pilz
Join Date: Feb 2017
Location: Leipzig, Germany
Posts: 590
Rep Power: 9 
> if you use large cells in the outer domain of your mesh and small cells near the surface there is always going to be a large difference between mean and max value of the Courant number
No, that is not the case. The Co number gives how many cells the flow moves in a time step. If the mesh is well balanced the flow moves around the same number of cells in every point of the mesh. > large difference between mean and max value of the Courant number. This does not mean you have a bad quality mesh. For not too complex simulations you may be right. But for complex situations an unnecessary fine mesh means unnecessary number of unknowns and therewith a system of equations which is less well conditioned. This may lead to numerical problems.
__________________
Uwe Pilz  Die der Hauptbewegung überlagerte Schwankungsbewegung ist in ihren Einzelheiten so hoffnungslos kompliziert, daß ihre theoretische Berechnung aussichtslos erscheint. (Hermann Schlichting, 1950) 

March 16, 2017, 12:27 

#13  
Senior Member

Quote:
Quote:
So I can not agree with you about this. 

March 16, 2017, 12:47 

#14 
Senior Member
Uwe Pilz
Join Date: Feb 2017
Location: Leipzig, Germany
Posts: 590
Rep Power: 9 
Dear Tom,
thank you for that explanation. Of course, they contain much trueness. But I believe here are other aspects to take in concern too. > The mesh needs to have correct spatial resolution to capture gradients in your flow. This seems to be true. But in reality you need the exact flow only in some regions of your problem. In the case of the wing you have to chose a spatial resolution in the near of the wing which covers the gradients, no questions. Normally, away from the wing the flow need only to solve to an accuracy which is adequate for covering the retroactive effects to the wing. It is not necessary to solve every detail of an eddy far away form the wing. So there you may have a coarser mesh. It may be a good strategy to make it at least as coarse as the balance of Co dictates: this leads to less time steps and to a more stable system of eqautions. > not true since you also get more equations for the unknowns Of course you get more equations. Without that you could not calculate the problem without any additional assumptions. But solving the system of equation means (in principle) to subtract a line of the system from the other as often as you have lines = unknowns. With more equations you get an accumulation of two bad effects: 1) Rounding errors increase. This leads slowly to less correct solutions 2) The probability that you have to subtract two nearly identical lines from each other increases. If that happens, you make something like division by zero (not full zero, but a very small number). In this case the solution gets wrong or explodes. The probability increases too, if you have cells which small changes in the flow variables in one part of the mesh and cells with rapid changes in another part. I know that the more advanced solvers don't simply subtract lines, but the principal problems remains. The chance to have a higher condition number increases with number of equations and with the differences in the Courant number (small changes against large ones).
__________________
Uwe Pilz  Die der Hauptbewegung überlagerte Schwankungsbewegung ist in ihren Einzelheiten so hoffnungslos kompliziert, daß ihre theoretische Berechnung aussichtslos erscheint. (Hermann Schlichting, 1950) Last edited by piu58; March 16, 2017 at 14:45. 

Tags 
convergance, openfoam, pimplefoam, relaxation factor, wing simulation 
Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Use homogeneous results as the initial guess for an inhomogeneous simulation  JuPa  CFX  5  December 26, 2014 14:44 
right settings and yPlus values for turbulent pipe simulation in OF  CRI_CFD  OpenFOAM PreProcessing  0  November 7, 2014 09:02 
Using the same simulation settings for new geometry  AHKB  STARCCM+  2  October 23, 2014 15:27 
Simulation and Optimisation of centrifugal fan 3D to 2D  eRzBeNgEl  STARCCM+  0  January 31, 2013 14:21 
3D Contaminant Dispersal Simulation  Apple L S Chan  Main CFD Forum  1  December 23, 1998 11:06 