
[Sponsors] 
September 30, 2011, 08:13 
Pressure instability with rhoSimpleFoam

#1 
New Member
Philipp Hofemeier
Join Date: Sep 2011
Location: Freiberg, Germany
Posts: 7
Rep Power: 7 
Dear all,
for my diploma thesis I am simulating a subsonic flow (Ma = 0.5) through a convergent divergent (De Laval) nozzle. For this purpose I choose to use the rhoSimpleFoam solver in OF 1.7.1. It works fine with some meshes. But on others it is not converging. To me it appears as if it is due to the aspect ratio for the cells. To show this I uploaded two identical cases. One has a high aspect ratio (a low resolution in flow direction → see the blockMeshDict). This mesh works fine and gives a good solution in comparison to theoretical calculations (http://dl.dropbox.com/u/24363809/Lav...soltion.tar.gz). The other has a low aspect ratio which means a high resolution in stream direction (http://dl.dropbox.com/u/24363809/Lav...soltion.tar.gz). Surprisingly this mesh does not converge although the mesh resolution is higher. The results show that the temperature and the velocity are quite stable and only the pressure is oscillating (as seen in the case folder). Besides the mesh the cases are completely identical. In order to solve the problem I tried several measures:
Non of these measures could stabilize the solution. All in all I would be grateful if somebody could help me solve the problem or explain why the rhoSimpleFoam solver cannot converge on the mesh with higher resolution. Furthermore, I would like to know if anybody ever used the rhoSimpleFoam solver on a tetrahedral mesh. Since I ran some calculation on different tetra meshes and all of them did not converge. Thanks for your help! Philipp 

October 3, 2011, 01:43 

#2 
Member

Hi phillip
use SonicFoam solver instead of rhosimplefoam. all we require is a compressible and turbulent solver. I fell like u will not get any issues with this solver Regards Kiran Ambilpur 

October 3, 2011, 06:10 

#3 
New Member
Philipp Hofemeier
Join Date: Sep 2011
Location: Freiberg, Germany
Posts: 7
Rep Power: 7 
Hello Kiran!
Thanks for your reply. However, to me the sonicFoam solver seems not to be the right solver for my problem. When you check the user guide it says that the sonicFoam is a "Transient solver for transsonic/supersonic, laminar or turbulent flow of a compressible gas". But I got a subsonic (and steady) problem to solve. Anyway, I will try it and let you know about my results. Philipp 

October 4, 2011, 13:22 

#4 
New Member
Philipp Hofemeier
Join Date: Sep 2011
Location: Freiberg, Germany
Posts: 7
Rep Power: 7 
Hi,
I tried the sonicFoam solver. By initialising "good" (fully converged) initial conditions the solver gives good results otherwise the solver needs long time to stabilize. However, the performance is not very good since I only need the steady state solution. Additionally, isn't sonicFoam an inviscid solver? For further applications I need to use a viscid solver. Has anybody some more experience with rhoSimpleFoam, especially on tetrahedral meshes? Regards, Philipp 

October 5, 2011, 02:56 

#5 
Senior Member
Christian Lucas
Join Date: Aug 2009
Location: Braunschweig, Germany
Posts: 200
Rep Power: 10 
Hi
it will be difficult getting a solution using a steady state solver for your problem. So my suggestion, don't spend more time on rhoSimpleFoam. About sonicFoam, I see no reason against this solver. You might want to consider changing the energy equation to a total energy equation, might increase stability. Solving the total energy equation If your simulations are too slow, try rhoPimpleFoam, but have a look at the continuity error and mass imbalance in your system. You should not relax the density and, in the last internal iteration, the pressure. About some of the points in your first post: "change of the discretization methods to limited, higher order schemes" > use upwind! "nonOrthogonalCorrectiors from 0 up to 10" > Do you have a strongly nonOrthogonal grid? If not, you don't need so many nonOrthogonalCorrectiors Best Regards, Christian 

October 5, 2011, 14:08 

#6 
New Member
Phil
Join Date: Mar 2011
Location: West Des Moines, Iowa, U.S.A.
Posts: 11
Rep Power: 7 
Philipp,
I took your LavalfineResolution case and ran it with version2.0.1. I was able to repeat the same behavior you observed. Then I dropped the relaxation factor on "rho" from 0.05 down to 0.01, and the solution converged. Note that I didn't change anything other than the relaxation factor for "rho". I've attached the fvSolution file and an image showing the convergence I obtained. I also tried to increase the relaxation factor on "rho" after it converged, and the residuals rose right back up to what you were observing with "rho 0.05;". I have no idea why the relaxation factor for "rho" should be so low... especially after the solution converges. Phil 

October 6, 2011, 09:44 

#7 
New Member
Philipp Hofemeier
Join Date: Sep 2011
Location: Freiberg, Germany
Posts: 7
Rep Power: 7 
Hey Phil,
I also observed the same behavior when I initialized a converged solution. But with a relaxation factor of 0.01 for rho seems to work well even on a tetra mesh! When I was playing with the relaxation factors I just changed the factors for p and U . So thank you very much! Regards, Philipp 

July 27, 2015, 09:31 

#8  
Member
Christa
Join Date: Apr 2011
Posts: 50
Rep Power: 7 
Quote:
I am struggling with rhoPimpleFoam at the moment, my pressure specifically will not converge (sum local = ~ 0.6) after trying several mesh resolutions, boundary conditions, fvSchemes and fvSolutions adjusted based on advice in this forum (mostly Gauss upwind schemes with GAMG solver for pressure), and the results I output before the simulation crashes look funny. I am very new to OpenFOAM and any advice (or directing me to another post on this forum I may have missed?) on things to look out for when using rhoPimpleFoam will be greatly appreciated. I am not posting my problem just yet because I know for a fact I have not tried everything yet. I am only looking for general tips. Thanks, Christa 

October 27, 2016, 02:23 

#9 
New Member
Harshal Akolekar
Join Date: Aug 2016
Location: Melbourne
Posts: 8
Rep Power: 2 
Hi Phil,
Thanks for your tip. My simulation with rhoSimpleFoam was also behaving strangely  oscillating. However, on reducing the residual of rho from 0.05 to 0.01  the solution is converging. Regards, Harshal 

October 29, 2016, 06:51 

#10 
New Member
Bo Kong
Join Date: Oct 2016
Location: China
Posts: 5
Rep Power: 2 
Hi phillip,
I also use rhoSimpleFoam to simulate a tansonic flow in a CD nozzel. But I meet some problems that an error reported: Maximum number of iterations exceeded I want to download your case file for help, but I cann't link the website you upload your file. Because the website is blocked... you know ,I am in China. So could send your case file to my mail:344500390@qq.com. Thanks! 

October 29, 2016, 23:31 

#11 
New Member
Harshal Akolekar
Join Date: Aug 2016
Location: Melbourne
Posts: 8
Rep Power: 2 
Hi Huangfei,
Make sure that all the equation variables have a relaxation factor defined for them.' This could be one of the issues. Please check it out. Regards, Harshal 

October 29, 2016, 23:34 

#12 
New Member
Harshal Akolekar
Join Date: Aug 2016
Location: Melbourne
Posts: 8
Rep Power: 2 
Hi Bo,
Please ensure that all the variables including h and e have relaxation factors defined for them in the fvSolutions file. Also check your BCs  make sure you are using stagation pressure BCs. Please check it out. Regards, Harshal 

October 30, 2016, 02:05 

#13 
New Member
Bo Kong
Join Date: Oct 2016
Location: China
Posts: 5
Rep Power: 2 
Hi Harshal,
Thanks for your reply. I solve that problem by revising the BC. But a new problem occurs. The residual of p is oscillating seriously after several iterations. Could you give some advice on this problem? 

October 30, 2016, 04:39 

#14 
New Member
Harshal Akolekar
Join Date: Aug 2016
Location: Melbourne
Posts: 8
Rep Power: 2 
Hi Bo,
What is the relaxation factor of rho. Make it around 0.01. I was also experiencing a similar problem. I reduced the relaxation factor of rho from 0.05 to 0.01  everything converged quite well after that. The pressure field also stopped oscillating. Hope it helps. Regards, Harshal 

Tags 
compressible flow, laval nozzel, rhosimplefoam, tetra mesh 
Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Calculation of the Governing Equations  Mihail  CFX  7  September 7, 2014 06:27 
Pulsatile pressure inlet with pressure outlet  a.lynchy  FLUENT  3  March 23, 2012 14:45 
Problem with rhoSimpleFoam : exploding enthalpy and density at the walls  david39  OpenFOAM Running, Solving & CFD  6  January 18, 2011 12:49 
Pressure in rhoSimpleFoam  vitor  OpenFOAM Running, Solving & CFD  2  September 16, 2010 11:49 
Setting pressure and velocity in inlet  Asghari  FLUENT  5  September 22, 2006 13:23 