
[Sponsors] 
chtMultiRegionSimpleFoam  Stabilise mass flux in a subdivided channel 

LinkBack  Thread Tools  Display Modes 
April 25, 2013, 06:42 
chtMultiRegionSimpleFoam  Stabilise mass flux in a subdivided channel

#1 
Member
Daniel Pielmeier
Join Date: Apr 2012
Posts: 96
Rep Power: 5 
When solving the flow through a subdivided channel the mass fluxes should be equal in all divisions. However the mass fluxes in the individual splits diverge from the expected distribution after some iterations.
Case geometry: geometry.jpg Starting from one inlet the channel is split up into eight separate channels (Here the mass flux is measured). Four of them are combined again to the two outlets. Mesh: detail.jpg The mesh consists of prismatic layers and a tetrahedra core mesh. The mesh seems coarse but this way I get quicker results. The problem occurs as well with a mesh triple the size. Output from checkMesh: log.checkMesh.txt Contents of fvSchemes and fvSolution for the fluid domain: fvSchemes.txt I have not a lot experience with different schemes so I just used the defaults from the heatTransfer/chtMultiRegionSimpleFoam/multiRegionHeater tutorial. Maybe there is room for improvement here. fvSolution.txt Here I already tried to lower the residual tolerances, add one NonOrthogonalCorrector and to underrelax a lot without success. Last edited by billie; April 25, 2013 at 16:12. 

April 25, 2013, 06:45 

#2 
Member
Daniel Pielmeier
Join Date: Apr 2012
Posts: 96
Rep Power: 5 
Adding further information in a second post as only five attachments are allowed per post.
Output from chtMultiRegionSimpleFoam: log.chtMultiRegionSimpleFoam.txt This is the output from the first iterations and some at iteration number 200. Mass flux of the different splits: mass_flux_splits.png Mass flux of the two outlets: mass_flux_outlet.png Is there a way to stabilise the system to avoid the divergence of the mass flux? 

April 25, 2013, 08:21 

#3 
New Member
Ignacio Gallego
Join Date: Jan 2013
Posts: 25
Rep Power: 4 
Hello Daniel,
The difference might be due to the asymmetry of the mesh. Why don't you create one half and then mirror the other? You just have to include a file called mirrorMeshDict. Also check the gravity direction! You are using a OneEquation turbulent model right? Why don't you change to a more accurate twoequation method? Cheers 

April 25, 2013, 08:55 

#4  
Member
Daniel Pielmeier
Join Date: Apr 2012
Posts: 96
Rep Power: 5 
Hello Ignacio,
thank you for your answer. Quote:
Gravity is applied in zdirection (the blue arrow from the coordinate system on the pictures) which should be fine. I would like to stick with SpalartAllmaras because I am comparing with another solver and the only turbulence model they have in common is this one. Last edited by billie; May 12, 2013 at 12:44. 

April 26, 2013, 03:53 

#5 
Member
Daniel Pielmeier
Join Date: Apr 2012
Posts: 96
Rep Power: 5 
I forgot to add some information about the boundary conditions applied.
At the inlet there is constant velocity and zeroGradient pressure. For the outflows there is zeroGradient velocity and constant pressure. 

April 28, 2013, 12:03 

#6 
Member
Daniel Pielmeier
Join Date: Apr 2012
Posts: 96
Rep Power: 5 
Nobody who can give me any hint here?
The mass flux on the inlet is 0.5kg/s so it should split to approximately 0.0625kg/s in the eight subdivisions and 0.25kg/s should reach the two outlets. From the charts in the second post one can see that the mass fluxes in the individual channels as well as in the outlets diverge completely. Split 14 get high and 58 even negative. The total mass balance is correct but the individual flows are unrealistic. I am trying to compare with another software which does not have this problem, so I think there must be anything wrong with my setup. 

May 14, 2013, 10:11 

#7 
Member
Daniel Pielmeier
Join Date: Apr 2012
Posts: 96
Rep Power: 5 
I found the reason for the extreme mass imbalance. If I increase the number of iterations the system balances after a high number of iterations. First of all refining the mesh and improving the mesh quality helps to some degree. The most influential factor however is relaxation. Until now I applied the same relaxation values for pressure and velocity. Lets say U = 0.6 and p = 0.6. Reducing both values only has the effect that it takes longer to converge but the imbalance remains the same. However underrelaxing velocity more than pressure greatly reduces the imbalance (U = 0.3, p = 0,7 like in the cht tutorial). There is still an initial imbalance but it is lower in magnitude and it takes a lot less iterations until the imbalance is resolved.


June 13, 2013, 13:28 

#8 
Member
Daniel Pielmeier
Join Date: Apr 2012
Posts: 96
Rep Power: 5 
I also played a bit with different schemes and found that using leastSquares as gradScheme and corrected as snGradScheme also reduces the imbalance as well as the simulation time. The individual iterations take longer but with the faster convergence the overall simulation time is reduced.


Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Fixed Outlet Mass Flux boundary condition?  trex930  OpenFOAM PreProcessing  2  June 30, 2010 21:44 
mass flux units in kg/ms  cfd~  Main CFD Forum  0  May 3, 2007 16:45 
Calcuationg mass flux of a UDS?  Derek  FLUENT  0  March 20, 2006 08:58 
mass flux correction at outflow boundaries  Subhra Datta  Main CFD Forum  2  November 24, 2003 14:11 
total mass flux correction for compressible fluid?  Francesco Di Maio  Main CFD Forum  0  August 21, 2000 04:23 