[rightnow]

Hi all I am a new user to OpenFOAM and I am trying to simulate flow in a cyclone device. This device is schematically shown in the first attached image. I have poor result of the simulation with the following settings:
1. solver - simpleFoam
2. mesh - tetrahedral, ~200 000 elements (geometry - Salome, mesh - Netgen)
3. turbulence model - kEpsilon, kOmegaSST
4.boundary conditions, fvSchemes, fvSolutions, yPlusRAS.log, checkMesh.log in attach *tar.gz file.
5. wall functions disabled because y+ <1

6. I using for first 50 iterations schemes first order (Gauss upwind), for next iterations - Gauss linearUpwind SquareLeast. I also tried to use potentialFoam.
Resuls of this simulation (shown in the second attached image) don't agree with the experimental setup finding (tangential velocity of the entire height of the device on average equal to 25-40 m / s).
How can I improve the simulation results?
Regards.

[markusrehm]

Hello,

you should try one of the RSM models (LaunderGibson) and improve mesh quality (maybe convert your mesh to a polyedral mesh). RSM tends to be less stable and the mesh will be more important.
Start with RSM on a converged kEpsilon solution.
Try limitedLinearV for velocity (similar to linearUpwind but for me it seemed to be more stable).

Markus

[rightnow]

Thanks for response
Tomorrow I will write about the results of simulations with RSM and limitedLinearV, but at the same mesh.
When I use to convert "polyDualMesh -concaveMultiCells", checkMesh gives a lot of mistakes and solution doesn't converge.
If I spend time creating structure mesh, I get a better result simulation? (example of the grid in attach image)

[arjun]

Originally Posted by rightnow

Thanks for response
Tomorrow I will write about the results of simulations with RSM and limitedLinearV, but at the same mesh.
When I use to convert "polyDualMesh -concaveMultiCells", checkMesh gives a lot of mistakes and solution doesn't converge.
If I spend time creating structure mesh, I get a better result simulation? (example of the grid in attach image)

If this is your mesh then you need much finer mesh to get it working. Cyclones are difficult to converge and your mesh is not helping much. Stick with structured mesh but refine it further.

[rightnow]

Sorry, I don't answer long time. I still havn't observe numerical simulation data, that are in good agreement with experiment.
Calculations are performed with structure hexa mesh (checkMesh in attach file) and turbulence model: kEpsilon, realizableKE, RNGkEpsilon, kOmegaSST, LRR, LaunderGibson.
Used the following case of fvSolution and fvSchemes.


fvSolution:
1. GAMG for pressure and smoothSolver with GaussSeidel for other
2. PCG for pressure and PBiCG for other


fvSchemes
1. upwind for div(p, U) and other div(x,x)
2. limitedLinearV for div(p,U) and upwind for other div(x,x)
3. linearUpwindV grad(U) for div(p, U) and linearUpwind grad(U) for other (p,U)
4. limitedLinearV grad(U) for div(p,U) and gamma 0,1 for other (p, U)


Boundary conditions:
1. velocity: inlet — 24,694 m/s, outlet — inletOutlet, wall — zeroGradient
2. pressure: inlet,wall — zeroGradient, outlet — 0
3. k: inlet 3/2*(0,05*U_inl)=2,2867, outlet and wall — zeroGradient, internalField — 2,2867
4. epsilon: for outlet and wall — zeroGradient, for inlet and internalField I consider two case:
4.1 epsilon=С_mu^(3/4)*k^(3/2)/l = 40,38
4.2 epsilon=k^(3/2)/(0,014*D)=1277,05 (recomendation from PhD Thesis S.Mauri: Numerical Simulation and flow analysis of an elbow diffuser)
5. R=(3/2k 0 0 3/2k 0 3/2k) = (3,43 0 0 3,43 0 3,43) for inlet and internalField, outlet and wall - zeroGradient

relaxationFactors set for uniform convergence each case.
20000-40000 iterrations
Modified files fvSolution and fvSchemes don't have much influence on results simulation.
Figure 1 shows the tangential velocity along the radius of the cyclone device (axis on the right, plot with "first" - upwind, with "second" - other schemes). Flow field isn't physically in all cases (in experiment: maximum tangential velocity — 45 m/s, and pick is locate at radius — 0,03 m).
Now I try numerical simulation with pisoFoam, but I think that will get the same values.

[markusrehm]

Hello,

I don't really understand the velocity plot.

What you could try:
-Think about a velocity profile at at the inlet or make the inlet longer so that a profile can develop.
-A fixed pressure at the outlet affects the profile close to it. Maybe a you should rather fix the pressure at a point close to the outlet. (See pRefValue in fvSolution).

You might also send your one fvSchemes-file as example.

Markus