# RhoSimpleFoam problem with patch

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 May 13, 2008, 10:06 Hi foamusers, I am tryin #1 Senior Member   Nishant Join Date: Mar 2009 Location: Glasgow, UK Posts: 165 Rep Power: 8 Hi foamusers, I am trying to run a compressible steady state problem with rhosimplefoam solver. The patches are something like this:- Inlet- pressure - fixedvalue 1.2 - velocity - pressureInletvelocity outlet - pressure - fixedvalue 1 - velocity - zerogradient After running for 3 time step, it stops abrupty like this: /home/343880/OpenFOAM/343880-1.4.1/run/tutorials/rhoExplicitPorousSimpleFoam Case : channel-mv-sy Nprocs : 1 Create time Create mesh for time = 0 Reading thermophysical properties Selecting thermodynamics package hThermo>>> > Reading field U Reading/calculating face flux field phi Creating turbulence model Selecting turbulence model laminar Starting time loop Time = 1 smoothSolver: Solving for Ux, Initial residual = 0.999941, Final residual = 0.0828475, No Iterations 2 smoothSolver: Solving for Uy, Initial residual = 0.999941, Final residual = 0.091559, No Iterations 2 smoothSolver: Solving for Uz, Initial residual = 1, Final residual = 0.0986704, No Iterations 2 DILUPBiCG: Solving for h, Initial residual = 0.435509, Final residual = 0.0101943, No Iterations 1 GAMG: Solving for p, Initial residual = 1, Final residual = 0.0436432, No Iterations 2 time step continuity errors : sum local = 3.80816e-05, global = -2.77424e-05, cumulative = -2.77424e-05 bounding p, min: 1.00109 max: 1.10057 average: 1.04803 rho max/min : 6.89377e-05 1.15862e-05 ExecutionTime = 0.43 s ClockTime = 0 s Time = 2 smoothSolver: Solving for Ux, Initial residual = 0.160346, Final residual = 0.0156449, No Iterations 2 smoothSolver: Solving for Uy, Initial residual = 0.432668, Final residual = 0.0365237, No Iterations 2 smoothSolver: Solving for Uz, Initial residual = 0.999207, Final residual = 0.0467854, No Iterations 4 DILUPBiCG: Solving for h, Initial residual = 1, Final residual = 0.0254643, No Iterations 1 GAMG: Solving for p, Initial residual = 1, Final residual = 0.0295425, No Iterations 3 time step continuity errors : sum local = 0.0499758, global = 0.00909272, cumulative = 0.00906498 bounding p, min: 16.5489 max: 60.9572 average: 30.2185 rho max/min : 0.000162646 1.15862e-05 ExecutionTime = 0.59 s ClockTime = 1 s Time = 3 smoothSolver: Solving for Ux, Initial residual = 0.365917, Final residual = 0.0183303, No Iterations 2 smoothSolver: Solving for Uy, Initial residual = 0.395495, Final residual = 0.0049005, No Iterations 4 smoothSolver: Solving for Uz, Initial residual = 0.387345, Final residual = 0.0231165, No Iterations 2 DILUPBiCG: Solving for h, Initial residual = 0.933419, Final residual = 0.0256051, No Iterations 1 #0 Foam::error::printStack(Foam:stream&) in "/home/343880/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libOpenFOAM.so" #1 Foam::sigFpe::sigFpeHandler(int) in "/home/343880/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libOpenFOAM.so" #2 Uninterpreted: [0x110420] #3 Foam::hThermo > > > >::calculate() in "/home/343880/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libbasicThermophysicalMo dels.so" #4 Foam::hThermo > > > >::correct() in "/home/343880/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libbasicThermophysicalMo dels.so" #5 main in "/home/343880/OpenFOAM/OpenFOAM-1.4.1/applications/bin/linuxGccDPOpt/rhoSimpleFo am" #6 __libc_start_main in "/lib/libc.so.6" #7 Foam::regIOobject::readIfModified() in "/home/343880/OpenFOAM/OpenFOAM-1.4.1/applications/bin/linuxGccDPOpt/rhoSimpleFo am" Floating point exception Can anybody suggest something? regards, nishant __________________ Thanks and regards, Nishant

 May 13, 2008, 10:21 Your pressure looks really rea #2 Senior Member   Mark Olesen Join Date: Mar 2009 Location: http://olesenm.github.io/ Posts: 777 Rep Power: 18 Your pressure looks really really low. (Do you have the correct units?) Unless you have a very modest resistance, you should also try the implicit formulation.

 May 13, 2008, 10:55 Hi Nishant You have a signi #3 Senior Member   Niels Gjoel Jacobsen Join Date: Mar 2009 Location: Deltares, Delft, The Netherlands Posts: 1,608 Rep Power: 25 Hi Nishant You have a significant continuity error, which I think originate from the fact, that you have a large residual in your solution to the pressure. Try to add one or two more iterations in the pressure. Hopefully that will help somewhat. - Niels __________________ Please note that I do not use the Friend-feature, so do not be offended, if I do not accept a request.

 May 13, 2008, 11:03 dimension for pressure is: di #4 Senior Member   Nishant Join Date: Mar 2009 Location: Glasgow, UK Posts: 165 Rep Power: 8 dimension for pressure is: dimensions [1 -1 -2 0 0 0 0]; which look okay to me. I tried my solver with higher pressure like 2, 3 , 11. but all failed in similar way. Nishant __________________ Thanks and regards, Nishant

 May 13, 2008, 11:32 Hi Neils .. Thanks for the re #5 Senior Member   Nishant Join Date: Mar 2009 Location: Glasgow, UK Posts: 165 Rep Power: 8 Hi Neils .. Thanks for the reply. how can I add more iteration to the pressure? can you tell me from where i can change the number of iteration? Nishant __________________ Thanks and regards, Nishant

 May 13, 2008, 12:08 Hi You can change it in #6 Senior Member   Niels Gjoel Jacobsen Join Date: Mar 2009 Location: Deltares, Delft, The Netherlands Posts: 1,608 Rep Power: 25 Hi You can change it in /case/system/fvSolution There is an entry called PISO, where you change the nCorrectors to a higher value. Here you can also set nonOrthogonalityCorrectors if needed. - Niels __________________ Please note that I do not use the Friend-feature, so do not be offended, if I do not accept a request.

 May 13, 2008, 12:34 Thanks Neils. Since its a #7 Senior Member   Nishant Join Date: Mar 2009 Location: Glasgow, UK Posts: 165 Rep Power: 8 Thanks Neils. Since its a steadystate solve, so there is SIMPLE instead of PISO. i change the ncorrectors to higher values like 4 for SIMPLE. but there is no effect on residual and simulation is still crashing after 3 time steps. Now the output is: Create mesh for time = 0 Reading thermophysical properties Selecting thermodynamics package hThermo>>> > Reading field U Reading/calculating face flux field phi Creating turbulence model Selecting turbulence model laminar Starting time loop Time = 1 smoothSolver: Solving for Ux, Initial residual = 1, Final residual = 0.0452055, No Iterations 4 smoothSolver: Solving for Uy, Initial residual = 1, Final residual = 0.0416017, No Iterations 4 smoothSolver: Solving for Uz, Initial residual = 1, Final residual = 0.0986704, No Iterations 2 DILUPBiCG: Solving for h, Initial residual = 0.525665, Final residual = 0.0347495, No Iterations 2 GAMG: Solving for p, Initial residual = 1, Final residual = 0.0436432, No Iterations 2 GAMG: Solving for p, Initial residual = 0.0199054, Final residual = 0.000583828, No Iterations 5 time step continuity errors : sum local = 11169.4, global = -5860.9, cumulative = -5860.9 rho max/min : 1.39034 1.15862 ExecutionTime = 0.48 s ClockTime = 1 s Time = 2 smoothSolver: Solving for Ux, Initial residual = 0.35641, Final residual = 0.00800959, No Iterations 2 smoothSolver: Solving for Uy, Initial residual = 0.448542, Final residual = 0.0159096, No Iterations 2 smoothSolver: Solving for Uz, Initial residual = 0.50882, Final residual = 0.00394456, No Iterations 2 DILUPBiCG: Solving for h, Initial residual = 1, Final residual = 0.087616, No Iterations 1 GAMG: Solving for p, Initial residual = 1, Final residual = 0.0303177, No Iterations 5 GAMG: Solving for p, Initial residual = 0.00260182, Final residual = 8.9025e-05, No Iterations 5 time step continuity errors : sum local = 1761.83, global = -720.736, cumulative = -6581.64 rho max/min : 2.66976e+07 1.15862 ExecutionTime = 0.7 s ClockTime = 1 s Time = 3 smoothSolver: Solving for Ux, Initial residual = 0.46346, Final residual = 0.0272365, No Iterations 2 smoothSolver: Solving for Uy, Initial residual = 0.489989, Final residual = 0.0350318, No Iterations 2 smoothSolver: Solving for Uz, Initial residual = 0.640354, Final residual = 0.0195653, No Iterations 2 DILUPBiCG: Solving for h, Initial residual = 1, Final residual = 0.052648, No Iterations 3 #0 Foam::error::printStack(Foam:stream&) in "/home/343880/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libOpenFOAM.so" #1 Foam::sigFpe::sigFpeHandler(int) in "/home/343880/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libOpenFOAM.so" #2 Uninterpreted: [0x110420] #3 Foam::hThermo > > > >::calculate() in "/home/343880/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libbasicThermophysicalMo dels.so" #4 Foam::hThermo > > > >::correct() in "/home/343880/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libbasicThermophysicalMo dels.so" #5 main in "/home/343880/OpenFOAM/OpenFOAM-1.4.1/applications/bin/linuxGccDPOpt/rhoSimpleFo am" #6 __libc_start_main in "/lib/libc.so.6" #7 Foam::regIOobject::readIfModified() in "/home/343880/OpenFOAM/OpenFOAM-1.4.1/applications/bin/linuxGccDPOpt/rhoSimpleFo am" Floating point exception Nishant __________________ Thanks and regards, Nishant

 May 13, 2008, 12:36 I even tried changing the tole #8 Senior Member   Nishant Join Date: Mar 2009 Location: Glasgow, UK Posts: 165 Rep Power: 8 I even tried changing the tolerance and relTol of the p. but that also didnt help. Nishant __________________ Thanks and regards, Nishant

May 14, 2008, 02:52
dimension for pressure is: d
#9
Senior Member

Mark Olesen
Join Date: Mar 2009
Location: http://olesenm.github.io/
Posts: 777
Rep Power: 18
Quote:
 dimension for pressure is: dimensions [1 -1 -2 0 0 0 0]; which look okay to me. I tried my solver with higher pressure like 2, 3 , 11. but all failed in similar way.
I didn't doubt the dimensions, since the solver would have complained immediately, but I've just never calculated any flow regimes with 1 Pascal pressure before. I think you should verify that the Navier-Stokes equations and/or the porosity model are actually valid at these pressures before you proceed any further.
What sort of Knudsen number do you have for this flow? Did you already add some rarified correction to the solver or is it unnecessary?

 May 15, 2008, 09:50 Thanks Mark, in fact we ar #10 Senior Member   Nishant Join Date: Mar 2009 Location: Glasgow, UK Posts: 165 Rep Power: 8 Thanks Mark, in fact we are planing to simulate the standing sound waves in these pressure ranges. Before that I felt that the solver is crashing with even fixedValue patch. The low pressure values are actually the relative pressures. But I tried running the case with totalPressure boundary condition as well and still the same result.! I have checked the navier stoke equation for the solver but how come I say that its valid or not? The Navier stokes equation is solving for convection, diffusion and laplacian terms and I am ok with that. Could you please tell me how to check the validity of the NS eqn? knudsen number is very low for these cases. Approx in range of 10-5 to 10-7. I tried some variation with the PISO corrector but they didnt help much. Nishant __________________ Thanks and regards, Nishant

May 16, 2008, 03:11
Nishant, From your explanat
#11
Senior Member

Mark Olesen
Join Date: Mar 2009
Location: http://olesenm.github.io/
Posts: 777
Rep Power: 18
Nishant,

From your explanation, what you are trying to do really doesn't fit together at all. You wish to specify a relative pressure, but I don't know how this is supposed to work with the rhoSimpleFoam solver. I can't see where the pressure datum should be comming from. From the output of the first iteration, it is quite evident that the pressure datum is indeed 0 Pa (ie, the rhoSimpleFoam is using absolute pressures):
Quote:
 bounding p, min: 1.00109 max: 1.10057 average: 1.04803 rho max/min : 6.89377e-05 1.15862e-05
For std. temp/pressure conditions, the density should be on the order of 1.
Changing to a thermodymamic pressure won't change much here.

Give what you are trying to simulate, I suspect you know a lot more about this field than I do. However, assuming a pressure datum of 100kPa, you should note that the pressure perturbations are at least 5 orders of magnitude smaller! An acoustic formulation, in which the perturbations are resolved directly, might prove more useful.
If the convective component is small and there are no large thermal gradients, the flank of the pressure waves might be shallow enough that a linearized acoustic solution might work. If the above assumptions are indeed true, a BEM or FEM method might be a better choice to consider. Unfortunately I know really nothing about acoustics per se, so I can't help you further. But if you do find a good solution, please let us know - it is a potentially really interesting area.

 May 20, 2008, 08:00 Thanks for the reply Mark. Sor #12 Senior Member   Nishant Join Date: Mar 2009 Location: Glasgow, UK Posts: 165 Rep Power: 8 Thanks for the reply Mark. Sorry for late. I am currently working with rhopSonicfoam to simulate my problem as it is a pressure-density based solver and most likely suitable for my problem. But my runs are repeatedly crashing around 0.49sec with high courant number. However its working quite fine with incompressible steady state solver simpleFoam. I therefore tried to run my case on rhoSimple foam, which is also a compressible steady state solver, to know whether it has something to do with time marching issues. I will soon try running it with rhosimplefoam case with suggestion u have given. I am also not sure about the pRefCell and prefValue. what value should i put for prefvalue for my case where i kept inlet boundary as totalpressure (104599pa). prefcell i took the first cell in outlet boundary of /constant/polymesh/boundary file. Is it ok? Nishant __________________ Thanks and regards, Nishant

 May 20, 2008, 08:25 Hi Nishant The specificatio #13 Senior Member   Niels Gjoel Jacobsen Join Date: Mar 2009 Location: Deltares, Delft, The Netherlands Posts: 1,608 Rep Power: 25 Hi Nishant The specification of pRefCell and pRefValue is only used if you are having gradient conditions on all boundaries, because the Poisson equation become non-unique if a level for the pressure is not specified. As long as you are specifying a pressure on the boundary, then pRefCell is not used. Best regards, Niels __________________ Please note that I do not use the Friend-feature, so do not be offended, if I do not accept a request.

 May 20, 2008, 10:13 Thanks Niels, This was very #14 Senior Member   Nishant Join Date: Mar 2009 Location: Glasgow, UK Posts: 165 Rep Power: 8 Thanks Niels, This was very helpful. Hi Mark, I am attaching my boundary condition files here please go through them and if you have some time then please try running it on either rhopSonicFoam or rhoSimpleFoam on your machine and let me know what you feel is going wrong. p U T Thanks in advance, Nishant __________________ Thanks and regards, Nishant

 May 22, 2008, 12:32 Hi Nishant I might have com #15 Senior Member   Niels Gjoel Jacobsen Join Date: Mar 2009 Location: Deltares, Delft, The Netherlands Posts: 1,608 Rep Power: 25 Hi Nishant I might have come around for a solution ... I have been trying for rather long time to solve one of the most classic problems, namely the Poiseuille flow, to test the calculation of my bed shear stresses. First I tried icoFoam, and it gave me significant problems when I specified pressure at both inlet and outlet, whereas gradient in p at inlet together with velocity field went succesfully. Trying different solvers, some succeeded and others gave rise to unbounded pressures. Finally I figured out that the momentum-correction before the PISO loop caused the instabilities, but in icoFoam and also in rhoSimpleFoam this momentum-correction is not controlled from the fvSolution-file, thus if you comment line 12 in ~/OpenFOAM/OpenFOAM-1.4.1/applications/solvers/compressible/rhoSimpleFoam/UEqn.H which looks like: solve(UEqn() == -fvc::grad(p)); you might get an improvement in your results. Some of you clever people out there would be very helpful, if you could explain why the momentum-correction causes such instabilities? Even more interesting would be to know when to use it? Thanks in advance and best regards. Niels __________________ Please note that I do not use the Friend-feature, so do not be offended, if I do not accept a request.

 October 30, 2009, 13:51 Shock wave with rhoSimpleFoam #16 Member   Sylvain Martel Join Date: Apr 2009 Location: University of Sherbrooke/Quebec/Canada Posts: 51 Rep Power: 8 Hi all, I am using rhoSimpleFoam solver to solve compressible air flow in a converging-diverging nozzle. Can this solver compute supersonic flow and take account for shock wave in the diverging part of the nozzle? The boundary condition are: To=573K Pin = 10e5 Pa Pout = variable Uin = PressureInletOutletVelocity = (0 0 0) Thank you very much Sylvain

 Thread Tools Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post matteo_gautero OpenFOAM Running, Solving & CFD 0 February 28, 2008 07:51 mattijs OpenFOAM Mesh Utilities 12 August 24, 2006 04:57 gzink OpenFOAM Running, Solving & CFD 0 August 3, 2006 13:50 massimo CD-adapco 1 February 24, 2003 22:23 Prateep Chatterjee FLUENT 1 April 11, 2000 06:04

All times are GMT -4. The time now is 09:48.

 Contact Us - CFD Online - Top