CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

simpleFoam + cyclone device. Poor result.

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree1Likes
  • 1 Post By rightnow

Reply
 
LinkBack Thread Tools Display Modes
Old   January 31, 2012, 01:20
Default simpleFoam + cyclone device. Poor result.
  #1
New Member
 
rightnow's Avatar
 
Andrey
Join Date: Jan 2012
Location: Russia, Severodvinsk
Posts: 3
Rep Power: 4
rightnow is on a distinguished road
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.
Attached Images
File Type: jpg cyclone.jpg (12.5 KB, 69 views)
File Type: jpg U_mag_YZ.jpg (17.8 KB, 64 views)
Attached Files
File Type: gz attach.tar.gz (71.6 KB, 21 views)
Bioksg likes this.
rightnow is offline   Reply With Quote

Old   February 1, 2012, 07:40
Default
  #2
Senior Member
 
Markus Rehm
Join Date: Mar 2009
Location: Erlangen (Germany)
Posts: 169
Rep Power: 7
markusrehm is on a distinguished road
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
markusrehm is offline   Reply With Quote

Old   February 1, 2012, 12:32
Default
  #3
New Member
 
rightnow's Avatar
 
Andrey
Join Date: Jan 2012
Location: Russia, Severodvinsk
Posts: 3
Rep Power: 4
rightnow is on a distinguished road
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)
Attached Images
File Type: jpg structure mesh.jpg (45.4 KB, 46 views)
File Type: png bad cells.png (5.8 KB, 39 views)
rightnow is offline   Reply With Quote

Old   February 1, 2012, 18:09
Default
  #4
Senior Member
 
Arjun
Join Date: Mar 2009
Location: Nurenberg, Germany
Posts: 353
Rep Power: 9
arjun is on a distinguished road
Quote:
Originally Posted by rightnow View Post
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.
arjun is offline   Reply With Quote

Old   March 4, 2012, 12:21
Default
  #5
New Member
 
rightnow's Avatar
 
Andrey
Join Date: Jan 2012
Location: Russia, Severodvinsk
Posts: 3
Rep Power: 4
rightnow is on a distinguished road
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.
Attached Images
File Type: png plot_all.png (11.1 KB, 60 views)
File Type: png LaunderGibsonRSTMSecondOrder_6.png (10.1 KB, 46 views)
File Type: png kOmegaSSTUpwind_1.png (7.7 KB, 44 views)
File Type: jpg de37dd9525b7ca6462ce3e6e394963f8.jpg (79.2 KB, 52 views)
Attached Files
File Type: gz checkMesh.tar.gz (1.2 KB, 14 views)

Last edited by rightnow; March 4, 2012 at 12:25. Reason: attach checkMesh.tar.gz
rightnow is offline   Reply With Quote

Old   March 5, 2012, 06:38
Default
  #6
Senior Member
 
Markus Rehm
Join Date: Mar 2009
Location: Erlangen (Germany)
Posts: 169
Rep Power: 7
markusrehm is on a distinguished road
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
markusrehm is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Laminar simpleFoam and inviscid simpleFoam herenger OpenFOAM Running, Solving & CFD 7 July 11, 2013 06:27
OpenFOAM compile error balkrishna OpenFOAM Installation 9 June 17, 2011 03:53
Compiling OpenFOAM on hpc-fe.gbar.dtu.dk kaergaard OpenFOAM Installation 1 June 16, 2011 01:33
Cyclone Simulation (simpleFoam) erncyc OpenFOAM 4 January 28, 2011 09:40
Modelling Industrial cyclone behaviour Gόnther Hasse Main CFD Forum 3 October 12, 1999 19:34


All times are GMT -4. The time now is 07:52.