
[Sponsors] 
BuoyantBoussinesqSimpleFoam and axialsymmetric results wrong mass flow 

LinkBack  Thread Tools  Display Modes 
December 14, 2009, 06:30 
BuoyantBoussinesqSimpleFoam and axialsymmetric results wrong mass flow

#1 
Member
Join Date: Apr 2009
Location: Karlsruhe, Germany
Posts: 96
Rep Power: 9 
Hallo all,
I have problems with the mass flow solving problems with buoyantBoussinesqSimpleFoamsolver. I'm solving axissymmetric flows with heat transfer, density changes can be neglected. The meshes are made with the blockMeshutility. The resiudals are very good (ca. 10e9). So as test case I solved an easy case with a heated pipe. Solving with the kepsilon turbulence model for different k, and epsilon show at the inlet wrong values. (inlet = 0.2917 0 0, gravity is in minus x1direction) In the diagramm you can see the inlet profil. So the massflow is wrong for the whole case (green and red, blue is good). So you can see, the values of the simulations show bad results, indeed a wrong massflow. Only neglecting gravity forces result the right inlet profil. Some steps afterwards: Solving this problem with simpleFoam (so no temperaturefield is beeing determinated, I get good results, indeed the same as solving with buoyantBoussinesqSimpleFoam without gravity: The two curves lie at the same positions: Solving a channelflow (not axissymmetric, but symmetric) I get very good results. So the wrong inletmassflow is only existing using buoyantBoussinesqSimpleFoam and axialsymmetric flowproblems. Has anybody an idea? Best regards, Thomas 

December 15, 2009, 05:07 

#2 
Member
Etienne Lorriaux
Join Date: Mar 2009
Location: Compiegne, France
Posts: 43
Rep Power: 9 
Hello,
how do you compute your mass flow and, what is your result and what is the radius of your pipe? I have already checked such things on axi cases and it was ok. edit: sorry I just saw the profiles after my answer. In fact, I think the main question is why are you getting such profiles while you are specifying an uniform velocity at inlet! I think there's something wrong in your postprocessing. Here is what I'm getting when I'm setting a uniform velocity at the inlet of an axi case: Etienne. Last edited by elorriaux; December 15, 2009 at 05:33. Reason: Pictures loaded after my answer 

December 18, 2009, 08:50 

#3 
Member
Join Date: Apr 2009
Location: Karlsruhe, Germany
Posts: 96
Rep Power: 9 
Hello,
for the plots in my first posting I used the sampledict using: interpolationScheme cell; type midPoint; I build some 3dmeshes, too. I got the same problems with the massflow. Using the postprocessingutility for the inlet or outlet boundary condition: (e.d. patchIntegrate phi inlet) and compare them with the theoretical (inletbulkvelocity*area) I get big differences if the gravity isn't zero. If there's no gravity the massflow results are very good, for axissymmetric and 3dmeshes. So I think the problem is the buoyantBoussinesqSimpleFoam solver. I wrote a new one without the hydrostatic pressure in the NavierStokesEquations. in createFields.H volScalarField deltarho ( IOobject ( "deltarho", runTime.timeName(), mesh ), beta*(T  TRef) ); in UEqn.H fvc::interpolate(deltarho)*(g & mesh.Sf()) instead of fvc::interpolate(rhok)*(g & mesh.Sf()) It was necessary to modify the pressurefile, that the residuals do converge, so in pEqn.H: surfaceScalarField buoyancyPhi = rUAf*fvc::interpolate(deltarho)*(g & mesh.Sf()); instead of: rUAf*fvc::interpolate(rhok)*(g & mesh.Sf()); The first simulations show the theoratical massflow. So for more informations about my simulations: I'm solving thermal turbulent liquidmetalflows with the buoancyBoussinesqSimpleFoam solver and RASmodels. The untypical conditions within these simulations are a high density (e.d. 11000kg/m^3) and the high thermal conductivity (e.d. Pr = 0.022). Regards Thomas Last edited by Thomas Baumann; December 19, 2009 at 07:38. 

December 18, 2009, 16:00 

#4 
Member
Etienne Lorriaux
Join Date: Mar 2009
Location: Compiegne, France
Posts: 43
Rep Power: 9 
Hello Thomas,
in fact, phi is not really the phi you are thinking in buoyantBoussinesqSimpleFoam. Look at pEqn.H, lines 11 to 13: surfaceScalarField buoyancyPhi = rUAf*fvc::interpolate(rhok)*(g & mesh.Sf()); phi += buoyancyPhi; So phi does not reflect velocity fluxes anymore and it is not the right value to use to compute flow rates. To be sure, I've just verified it on a small test case, with density = 11000 kg/m3, gravity = 9.81 m/s2 normal to the inlet patch. patch area = 0.0040438 m2 imposed velocity = 0.4 m/s so imposed flow rate should be 0.00161752 m3/s (add a minus for surface orientation) patchIntegrate phi inlet = 0.00125536 m3/s patchIntegrate buoyancyPhi = 0.000362164 m3/s So effectively, integrating phi shows 22% error on the flow rate, but integrating (phi  buoyancyPhi) gives 0.001617524 m3/s. It looks good to me Regards, Etienne. 

December 21, 2009, 04:42 

#5 
Member
Join Date: Apr 2009
Location: Karlsruhe, Germany
Posts: 96
Rep Power: 9 
Hello Etienne,
thank you very much for your hinds. I have calculated the massflow of the 3dcase in another way: I calculated the velocitymagnitude and calculated the massflow (neglecting density changes) foamCalc mag U patchIntegrate magU inlet patchIntegrate magU outlet for no gravity: inlet: 0.000408379 m^3/s oulet 0.000408379 m^3/s gravity in flow direction: inlet: 0.00040379 m^3/s oulet: 0.000463418 m^3/s gravity in minus flow direction: inlet: 0.00040739 m^3/s outlet: 0.000362151 m^3/s So the outflowrate depends on the gravitytensor using the velocityfield and not the phifield. The massflow isn't constant over the hole pipe. Or is a part of the massflow in the buoyancyPhi and I have to correct my velocityfield for postprocessing? Regards Thomas 

December 21, 2009, 07:57 

#6 
Member
Etienne Lorriaux
Join Date: Mar 2009
Location: Compiegne, France
Posts: 43
Rep Power: 9 
Hello Thomas,
I can't really be more helpful since I can't see the same behavior on my case. Integrating U gives the right flow rate on my case. What about the convergence? It's suspicious to get such errors on the flow rate if the continuity convergence is OK. Which values are you using for beta and TRef? What is the mean value of your temperature field? Are you still in good agreement with the boussinesq assumption? Regards, Etienne. 

December 21, 2009, 11:31 

#7 
Member
Join Date: Apr 2009
Location: Karlsruhe, Germany
Posts: 96
Rep Power: 9 
Hi Etienne,
the residuals are good. Uy, Ux, Uz, epsilon, p , T and k < 10e7. time step continuity errors : sum local = 1.3705e08, global = 4.21107e10, cumulative = 2.44451e05 So I think they should be good enough. For beta I'm using 0.000128. The inlettemperature is about 573 K, the same as the reference temperature. Temperature changes are smaller than 50 K, so density changes are smaller than 0.5 percent. I think you can use here the boussinesq assumption. I'm solving the problem with the modified solver now, because here is the massflow okay and I don't need the hydrostatic pressure for my calculations. I need some results in January... But I'm still trying to find the mistake or whatever. So thanks a lot and best regards, Thomas 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
How to Monitor Mass flow rate in CFX  Md Hamidur  CFX  13  November 6, 2015 23:34 
mass flow convergence on interfaces  Tatiana  STARCCM+  0  June 25, 2009 03:19 
Axial flow turbine approperiate B.C  dia aisa  CFX  0  April 30, 2008 03:32 
some weird results about a simple pipe flow:  Ning  FLUENT  2  March 11, 2007 14:23 
Target mass flow rate  Saturn  FLUENT  0  December 10, 2004 05:18 