
[Sponsors] 
Blow of compressible solver while using Kepsilon model in openfoam 

LinkBack  Thread Tools  Display Modes 
January 25, 2011, 07:57 
Blow of compressible solver while using Kepsilon model in openfoam

#1 
New Member
Amit Mathur
Join Date: Dec 2010
Location: India, New Delhi
Posts: 10
Rep Power: 8 
Dear all,
I am trying to run a simulation for a compressible flow in a pipe by using the KEpsilon turbulence model in the version 1.7 from OpenFOAM. For this simulation, I use a compressible solver : rhoSimpleFoam and I have defined the following boundary conditions :  Inlet : pressure101325  Outlet : pressure98383 My problem is that, after some iterations, the epsilon start bounding for very high values like 1e70. Afterwards solver blow and stop working. I used Kepsilon, resizable Kepsilon, RngKE but problem remain as it is. I already have remeshed my geometry to try to get a better mesh (orthogonal cell at the walls) but the problem persists. I already have increased the number of nNonOrthogonalCorrectors but the problem persists. To reproduce my problem, I have meshed a straight pipe and used the same setup. With the straight pipe (hexahedra), there is no problem and with a complex geometry (hexcore mesh from Tgrid), I do not understand what happens. I presume that there are some problems with my setup but I do not understand where. Afterwards i applied KOmegaSST model. That time solver produce results but i dont why Kepsilon is not running. So my question is why Kepsilon model in compressible flow is not working with Tet mesh in openfoam? Thanks. Best regards, Amit 

January 26, 2011, 11:35 

#2 
Senior Member
Nakul
Join Date: Apr 2010
Location: India
Posts: 147
Rep Power: 8 
Hi,
It seems possible that there might be some problem with your BC. Do you really need a fixed value of pressure at outlet? Try changing outlet pressure to zeroGradient, What is the flow velocity and temperature? Specify more details of your case. 

January 27, 2011, 01:06 
problem in rhosimplefoam using kepsilon model

#3 
New Member
Amit Mathur
Join Date: Dec 2010
Location: India, New Delhi
Posts: 10
Rep Power: 8 
Hi nakul,
Thanks for reply. Flow in the geometry is pressure driven so the inlet at higher pressure and outlet at lower pressure. The velocity bc is zero gradient at both outlet and inlet. The temperature is fixed at 293 K for both inlet and outlet. I tried the same BC for hex mesh it works properly for Kepsilon model but in Tet mesh its fail even mesh quality is good. 

January 27, 2011, 02:30 

#4 
Senior Member
Nakul
Join Date: Apr 2010
Location: India
Posts: 147
Rep Power: 8 
Hi,
Do a checkMesh on your tet mesh and see what you get. Try reducing Co no. and use first order schemes in fvSchemes. See if is helps. 

January 27, 2011, 03:28 
problem in rhosimplefoam using kepsilon model

#5 
New Member
Amit Mathur
Join Date: Dec 2010
Location: India, New Delhi
Posts: 10
Rep Power: 8 
Dear Nukul,
I am using steady compressible solver (rhoSimpleFoam), there is no need of co no. I am sending you the cheak Mesh result. Ots seems to be Ok. Thanks Checking geometry... Overall domain bounding box (0.917934 0.649145 0.434051) (0.147203 0.0148634 0.759144) Mesh (nonempty, nonwedge) directions (1 1 1) Mesh (nonempty) directions (1 1 1) Boundary openness (9.87366e16 8.81665e17 3.83878e17) OK. Max cell openness = 7.52033e16 OK. Max aspect ratio = 38.487 OK. Minumum face area = 9.7289e09. Maximum face area = 0.00235134. Face area magnitudes OK. Min volume = 2.21352e12. Max volume = 0.000103724. Total volume = 0.0505074. Cell volumes OK. Mesh nonorthogonality Max: 71.3198 average: 22.1898 *Number of severely nonorthogonal faces: 1. Nonorthogonality check OK. <<Writing 1 nonorthogonal faces to set nonOrthoFaces Face pyramids OK. Max skewness = 3.35511 OK. 

January 27, 2011, 03:38 

#6 
Member
Join Date: Jun 2010
Posts: 33
Rep Power: 8 
Hi,
I tried for two months rhoSimpleFoam, wasn't easy to get a stable simulation. Right settings in fvSchemes and fvSolution are very important. relTol, relaxationFactors, divSchemes In my opinion try to set: fvSolution: solvers { ... relTol 0.1; ... } relaxationFactors { p 0.01; rho 0.01; U 0.5; h 0.1; k 0.1; epsilon 0.1; } When it works, you could set the factors higher. fvSchemes: divSchemes { div(phi,U) Gauss vanLeerV; div(phi,k) Gauss upwind; div(phi,epsilon) Gauss upwind; } I would use realizable kEpsilon. Are your velocity high? Why you have fixed temperature at inlet and outlet? Regards, Ralph 

January 27, 2011, 05:36 
problem in rhosimplefoam using kepsilon model

#7 
New Member
Amit Mathur
Join Date: Dec 2010
Location: India, New Delhi
Posts: 10
Rep Power: 8 
Dear RalpS,
Thanks for replying. I adjust the system schemes, solution and relaxation factor according to you. But the problem is same the solution stops for KE. Well resizable KE is already running successfully but it is not converging. While using KOmega SST model the solution is converged and max Velocity is 130m/s. For KEpsilon the problem is remain as its is Thanks
__________________
It is not in the stars to hold our destiny but in ourselves
Regards Amit Mathur 

January 27, 2011, 06:08 

#8 
Member
Join Date: Jun 2010
Posts: 33
Rep Power: 8 
Have your tried to use a start solution for KE?
With realizable KE and KOmega SST the simulation runs without stopping? Why you want to use KE then? 

January 27, 2011, 06:14 
problem in rhosimplefoam using kepsilon model

#9 
New Member
Amit Mathur
Join Date: Dec 2010
Location: India, New Delhi
Posts: 10
Rep Power: 8 
Dear RalpS,
The solution runs successfully in Simple Foam (incompressible) but fails using rhoSimpleFoam (compressible) while using Kepsilon. The initial value of KE from turbulent intensity and mixing length.
__________________
It is not in the stars to hold our destiny but in ourselves
Regards Amit Mathur 

January 28, 2011, 03:59 

#10 
Senior Member
Nakul
Join Date: Apr 2010
Location: India
Posts: 147
Rep Power: 8 
Hi Amit,
Since you are getting converged solutions with komega that means your case setup is correct. But if you want to have solutions with kepsilon try the following and see if you are getting any convergence: 1 Are you using the fvSchemes proposed by Ralph? If yes then make the divScheme for (phi, U) as upwind also. Use upwind scheme for all divSchemes as it is first order. 2 Run the case with turbulence switched off and solve for the flow field. Then use this converged solution as initial condition for turbulence on. Hope this helps you. If you still face problems then upload your case and I will try to have a look if time permits. 

January 28, 2011, 05:10 

#11 
Senior Member
Olivier
Join Date: Jun 2009
Location: France, grenoble
Posts: 266
Rep Power: 10 
Hello,
Did you run in parallel ? Because there is some trouble with turbulence (kepsilon) and DILUPBiCG (see http://www.cfdonline.com/Forums/ope...tml#post246561 ) So you may try to switch to smooth solver for U, k and epsilon, and keep Gauss upwind for div(phi,k) and div(phi,epsilon) Also try Gauss linearUpwind cellLimited Gauss linear 1; for div(phi,U) Regards, olivier 

January 28, 2011, 06:29 
problem in rhosimplefoam using kepsilon model

#12 
New Member
Amit Mathur
Join Date: Dec 2010
Location: India, New Delhi
Posts: 10
Rep Power: 8 
Hi Nukul,
Thanks for replying. I made changes what so ever you suggested to me. But the problem is remain as it is. The solution blow of after some iterations. It runs good while making turbulence off and starts converging. I solve the flow field without turbulence model. Its runs and converged up to 10e3. And then "on" the turbulence model. But again solution is blow after 9 or 10 iterations. Thanks
__________________
It is not in the stars to hold our destiny but in ourselves
Regards Amit Mathur 

January 28, 2011, 06:34 

#13 
Senior Member
Olivier
Join Date: Jun 2009
Location: France, grenoble
Posts: 266
Rep Power: 10 
Hello,
OpenFoam is sensitive to initial values, specialy with turbulence one. Show your k and epsilon file in 0/ dir. What is your initial conditions ? Regards, olivier 

January 28, 2011, 06:59 
problem in rhosimplefoam using kepsilon model

#14 
New Member
Amit Mathur
Join Date: Dec 2010
Location: India, New Delhi
Posts: 10
Rep Power: 8 
Hi OlivierG,
Thanks for reply. I runs solver in parallel. But in series the problem of blowing is not solved. I changed the solver and schemes settings as you suggest to me but the problem as its is. Here below i am showing my k and epsilon file. K FoamFile { version 2.0; format binary; class volScalarField; location "0"; object k; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [ 0 2 2 0 0 0 0 ]; internalField uniform 1; boundaryField { wall { type compressible::kqRWallFunction; value uniform 1; } inlet { type turbulentIntensityKineticEnergyInlet; intensity 0.01; value uniform 1; } outlet { type inletOutlet; inletValue uniform 1; value uniform 1; } symplane { type symmetryPlane; } } and Epsilon dimensions [0 2 3 0 0 0 0]; internalField uniform 1; boundaryField { inlet { type fixedValue; value uniform 1; } outlet { type fixedValue; value uniform 1; } symplane { type symmetryPlane; } wall { type compressible::epsilonWallFunction; value uniform 1; } }
__________________
It is not in the stars to hold our destiny but in ourselves
Regards Amit Mathur 

January 28, 2011, 07:15 

#15 
Senior Member
Olivier
Join Date: Jun 2009
Location: France, grenoble
Posts: 266
Rep Power: 10 
Hello,
1) for outlet, try zeroGradient for k and epsilon 2) for inlet, k is ok, but for epsilon you can use "turbulentMixingLengthDissipationRateInlet" In any case, for k/epsilon, you may also try fixedValue at inlet 3) You use initial value 1 for k and 1 for epsilon: are you sure this is a correcte estimation ? (i think no) check http://www.openfoam.com/docs/user/ca...#x5290002.1.7 at chap2.1.8.1 Regards, Olivier 

January 29, 2011, 03:46 
problem in rhosimplefoam using kepsilon model

#16 
New Member
Amit Mathur
Join Date: Dec 2010
Location: India, New Delhi
Posts: 10
Rep Power: 8 
Dear OlivierG,
Thanks for reply. I made the k and epsilon boundary condition to zero gradient at outlet and for inlet epsilon turbulentMixingLengthDissipationRateInlet is used. The mixing length is 0.00821. It is difficult to predict the correct value of kepsilon for boundaries because the flow is pressure driven. Inlet101325 outlet98383 But on the basis of successful simulation of model using KomegaSST model which is previously done. The max velocity is 130m/s. As reference of that velocity 130m/s and using intensity 1% i calculate k=2.535 and epsilon=4.368. But the things are not working, the solution is just blow off after 5 iterations. thanks
__________________
It is not in the stars to hold our destiny but in ourselves
Regards Amit Mathur 

October 6, 2013, 11:09 

#17  
Member
Martin Novák
Join Date: Dec 2012
Location: Prague
Posts: 56
Rep Power: 6 
Quote:
I am facing same issue. Did you find out a reasonable solution for such a setting? Best regards Martin 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Weller combustion model  engineFoam solver.  ghindi  OpenFOAM Running, Solving & CFD  1  May 6, 2016 05:56 
compressible flow calculation error using rhoSimpleFoam solver  student4326  OpenFOAM Running, Solving & CFD  7  November 2, 2015 12:34 
bounding epsilon blow up  jiez  OpenFOAM Running, Solving & CFD  4  January 16, 2011 18:14 
Epsilon boundary condition for walls in LamBremhorst LowRe model  maruthamuthu_venkatraman  OpenFOAM  0  March 16, 2010 04:27 
Compressible magnetohydrodynamics solver  thekay  OpenFOAM  0  January 27, 2010 09:04 