
[Sponsors] 
pressure eq. "converges" after few time steps 

LinkBack  Thread Tools  Search this Thread  Display Modes 
February 9, 2011, 06:41 

#61 
Senior Member

So, results for
1. Uncorrected 2. Limited 0.333 3. Limited 0.5 4. Limited 0.667 5. Corrected Uncorrected.pngLimited_0.333.pngLimited_0.5.pngLimited_0.667.pngCorrected.png !!! Stair type of the plot is used to distinguish iteration values better, not the numerical behavior !!!
__________________
Best regards, Dr. Alexander VAKHRUSHEV Christian Doppler Laboratory for "Metallurgical Applications of Magnetohydrodynamics" Simulation and Modelling of Metallurgical Processes Department of Metallurgy University of Leoben http://smmp.unileoben.ac.at Last edited by makaveli_lcf; February 9, 2011 at 07:00. 

February 18, 2011, 08:23 

#62 
Senior Member

Another issue that I found:
I plotted the pressure residuals for my pimpleFoam solution (see Fig). p_resid_relax_p=0.3_U=0.7.png schemes are gradSchemes: cellLimited leastSquares 1; div: upwind laplacian and surface gradients: Gauss linear limited 0.5; limited 0.5; Initial underrelaxation parameters: Code:
p 0.3; U 0.7; I fought with it varying underrelaxation parameters, increasing the step number of the corrections (outer, neighbor and nonorthogonality) ; changed the used schemes to fully corrected and removed cell limiting; reduced Courant number to < 1.... Nothing from those helped! Sudden solution was to REMOVE THE UNDERRELAXATION OF THE MOMENTUM EQUATION ! p_residual_fixed.png Why is it so, I have now explanation! The whole advantage of the underrelaxation is vanished! For the clarification, final working settings, which removed residuals jump are: Code:
relaxationFactors { p 0.2...0.8; // For higher values solution diverges (Co ~ 4) U 1; } a) As I understood, in FLUENT relaxation is applied only for the fields (please correct me if I am wrong!). Here in OF's PIMPLE as well as in PISO and SIMPLE algorithms, it is "field underrelaxation" being applied for the pressure versus "matrix underrelaxation" for the momentum equation to increase its diagonal dominance. In presented case according to my observations momentum underrelaxation makes no sense.... b) Is there any way to get initial residuals not solving the linear system in OF? As far as I know, Solver Performance Class returns required information regarding residuals only by means of the "solve" method... Setting maxIter parameter to 0 for the linear solver does not help! BTW, Franco, thanks a lot for indicating this solver parameter, it is rather useful!))) Regards to all... And may the Source be with you!))) Alexander
__________________
Best regards, Dr. Alexander VAKHRUSHEV Christian Doppler Laboratory for "Metallurgical Applications of Magnetohydrodynamics" Simulation and Modelling of Metallurgical Processes Department of Metallurgy University of Leoben http://smmp.unileoben.ac.at 

March 8, 2011, 05:24 

#63 
Member
Vishal Jambhekar
Join Date: Mar 2009
Location: University Stuttgart, Stuttgart Germany
Posts: 90
Blog Entries: 1
Rep Power: 17 
Hi All,
I am also trying to do flow simulation for a city model. And using Simplefoam form the same. I am also facing similer kind of issues as MALLALENA please rever to following post for case details. http://http://www.cfdonline.com/For...urbulence.html I was thinking it is due to inlet conditions but I found out that the pressure solwing is getting blown up after few iterations. I am using tetrahedral mesh. Thanks a lot for ur kind help
__________________
Cheers, Vishal Jambhekar... "Simulate the way ahead......!!!" 

March 8, 2011, 05:30 

#64 
Member
Vishal Jambhekar
Join Date: Mar 2009
Location: University Stuttgart, Stuttgart Germany
Posts: 90
Blog Entries: 1
Rep Power: 17 
Hi All,
I am also trying to do flow simulation for a city model. And using Simplefoam form the same. I am also facing similer kind of issues as MALLALENA please rever to following post for case details. http://http://www.cfdonline.com/For...urbulence.html I was thinking it is due to inlet conditions but I found out that the pressure solwing is getting blown up after few iterations. I am using tetrahedral mesh. Thanks a lot for ur kind help
__________________
Cheers, Vishal Jambhekar... "Simulate the way ahead......!!!" 

March 8, 2011, 10:32 

#65  
Member
Vishal Jambhekar
Join Date: Mar 2009
Location: University Stuttgart, Stuttgart Germany
Posts: 90
Blog Entries: 1
Rep Power: 17 
Quote:
Similar situation is happening for me. The solution blows up after some time steps. I also have bonding values for K and epsilon. Can you please tell me what did you do to make solution stable. I have also reduced relaxation factor an reltol (0.05) but still not working. Please let me know...
__________________
Cheers, Vishal Jambhekar... "Simulate the way ahead......!!!" 

March 10, 2011, 02:36 

#66  
Senior Member
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 23 
Hello,
what does this mean? Quote:
Otherwise, you may have bad cells (what checkmesh says?) or schemes which are not good, thus you have to play a bit with them. In any case:
mad 

March 10, 2011, 04:13 

#67 
Member
Vishal Jambhekar
Join Date: Mar 2009
Location: University Stuttgart, Stuttgart Germany
Posts: 90
Blog Entries: 1
Rep Power: 17 
Hi Maddalena,
My apologies for inconvinience. Can you please help me a bit. I think you have already figured out the way for stable solution. my case details are posted here. http://www.cfdonline.com/Forums/ope...urbulence.html I have also attached check mesh log in the same thread. Thanks a lot for ypur help VJ
__________________
Cheers, Vishal Jambhekar... "Simulate the way ahead......!!!" 

July 21, 2011, 06:49 

#68 
New Member
Joel Lehikoinen
Join Date: Jun 2011
Posts: 26
Rep Power: 15 
This is an old topic, but I think it is still of interest to many, so I'll post my findings on the subject here. I had some trouble getting a buoyantPimpleFoam test case to converge, but in the end, I think I managed to get it to converge nicely. I will first describe the case in detail, and then outline the steps I took to improve convergence and accuracy.
I was simulating a simple case of pipe flow in a circular pipe with mesh of just 80000 cells. The solver used here is buoyantPimpleFoam. The flowing fluid is water, initially at temperature of 10 C. I used the icoPoly8 thermodynamics package, with coefficients obtained by fitting a curve to thermophysical property data from NIST webbook. Diameter of the pipe is 140 mm and its length is 1070 mm. The flow velocity at inlet is 0.5 m/s in the positive xaxis direction. The flow is turbulent (Re 10600), and the turbulence model used was the standard kepsilon. The boundary conditions were set followingly: U: Code:
Inlet: fixed velocity at 0.5 m/s Outlet: pressureInletOutletVelocity Wall: fixed 0 m/s (noslip) Code:
Inlet: buoyantPressure Outlet: fixed 10000 Pa Wall: zeroGradient Code:
Inlet: fixed 283 K Outlet: zeroGradient Wall: fixed 350 K Attached you will find my fvSolution and fvSchemes files, as well as a plot of initial residuals vs. time. I made some changes during runTime to these files, which can be seen in the plot. First I played around a bit with the underrelaxation coefficients, but unfortunately I didn't document what I did exactly.
In conlusion, at least for the case in question we found out that:


July 21, 2011, 07:29 

#69 
Senior Member
Felix L.
Join Date: Feb 2010
Location: Hamburg
Posts: 165
Rep Power: 18 

July 21, 2011, 07:42 

#70 
Senior Member
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 23 
that is the right way of doing things in OpenFOAM: sharing experience! thank you to have joined in this thread!


Tags 
convergence issues, pipe flow, simplefoam 
Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
TimeVaryingMappedFixedValue  irishdave  OpenFOAM Running, Solving & CFD  32  June 16, 2021 06:55 
time Step's turbFoam >>> exit  mgolbs  OpenFOAM PreProcessing  4  December 8, 2009 03:48 
Modeling in micron scale using icoFoam  m9819348  OpenFOAM Running, Solving & CFD  7  October 27, 2007 00:36 
Hydrostatic pressure in 2phase flow modeling (CFX4.2)  HB &DS  CFX  0  January 9, 2000 13:19 
unsteady calcs in FLUENT  Sanjay Padhiar  Main CFD Forum  1  March 31, 1999 12:32 