
[Sponsors] 
October 29, 2013, 17:05 
buoyantSimpleFoam and watertank

#1 
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Tussenhausen
Posts: 2,679
Blog Entries: 6
Rep Power: 49 
Dear Foamers,
I am working (since 2 weeks) on a very simple simulation. What I want to simulate: Something like that: http://www.wigaenergietechnik.de/bi...mage/lwsp2.gif What I did:  I meshed the whole geometry with a corse and very fine mesh  I build polynoms for water thermodynamics (30°C70°C)  I changed the thermodynamics for water  Simulation is LAMINAR  Inlet 4e5 m³/s  At the inlet I have a very simple pipe installation but the solver blow up every time so I just set an Inlet + Outlet (thats all  see pictures). Now my problem: Every BC I set make problems. I am not 100% sure how I should set the p_rgh BC for inlet/outlet/wall. p is calculated. For U and T its clear. The solver is working just for 1 or none iterations. If I set of the gravity the simulation is working. It seems that the solver is calculating my water with a compressibility because after the first time step I get extrem huge velocity fields in the big domain. I tried a lot of BC for U + p_rgh  fixed at the outlet  pressureInletOutletVelocty etc. Does someone can give me a hint how to set these BC right? Relaxationfactors are decreased to 0.1. linearUpwind + limitedLinear schemes are used etc... Interesting fact: without gravitation the simulation is working. With gravitation the mass flux cant be calculated: Code:
> FOAM FATAL ERROR: Continuity error cannot be removed by adjusting the outflow. Please check the velocity boundary conditions and/or run potentialFoam to initialise the outflow. Total flux : 102320 Specified mass inflow : 0.29563 Specified mass outflow : 0.151702 Adjustable mass outflow : 0 The error message: Code:
Time = 2 DILUPBiCG: Solving for Ux, Initial residual = 0.733571, Final residual = 0.0031127, No Iterations 7 DILUPBiCG: Solving for Uy, Initial residual = 0.623405, Final residual = 0.000739902, No Iterations 8 DILUPBiCG: Solving for Uz, Initial residual = 0.701814, Final residual = 0.0023944, No Iterations 7 DILUPBiCG: Solving for h, Initial residual = 1, Final residual = 0.00132406, No Iterations 2 > FOAM FATAL ERROR: Maximum number of iterations exceeded From function thermo<Thermo, Type>::T(scalar f, scalar T0, scalar (thermo<Thermo, Type>::*F)(const scalar) const, scalar (thermo<Thermo, Type>::*dFdT)(const scalar) const, scalar (thermo<Thermo, Type>::*limit)(const scalar) const) const in file /home/shorty/OpenFOAM/OpenFOAM2.2.x/src/thermophysicalModels/specie/lnInclude/thermoI.H at line 76. FOAM aborting Any suggestions would be appreciated. Regards Tobi 

October 30, 2013, 03:55 

#2 
Member
hannes
Join Date: Mar 2013
Posts: 47
Rep Power: 11 
Hi Tobi,
seems to me as your problem might arise due to the initial conditions of p. In your final solution the p field should be close to the hydrostatic field and p_rgh close to constant. However, if you assume p to be constant in the beginning then you get the p_rgh field shown in your plot which leads to high velocities and possibly even to a crash. The problem is that in the very first step the solver uses the pfield to calculate the p_rgh field although your boundary conditions are set for p_rgh and p is set to calculated. So what you can do is either adapt the solver (which is just a change of one line) or probably a little bit easier use funkySetFields to set the initial pressure field to the hydrostatic pressure. Hope that helps Hannes 

October 30, 2013, 05:41 

#3 
Senior Member

Hi Tobi,
As a bypass you could run initially with gravity turned off. Than after say 200 iterations turn gravity on. Unfortunately it is not runtime modifiable so you have to stop (and save) the run, change gravity and rerun from latestTime. Regards, Tom 

October 31, 2013, 05:24 

#4 
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Tussenhausen
Posts: 2,679
Blog Entries: 6
Rep Power: 49 
Hi,
thanks for your replays. I tried Toms hints. The pictures show p, p_rgh and U after 500 iterations. Then i turned gravity on and the 501 step is shown in the 2nd replay. @hannes: what lines had to be modified? @all: could it be possible that my polynomes are wrong? Last edited by Tobi; October 31, 2013 at 08:41. 

October 31, 2013, 05:49 

#5 
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Tussenhausen
Posts: 2,679
Blog Entries: 6
Rep Power: 49 
Here are the pictures at 501 iterations.
After that my solver blow up: Code:
[5] [5] [5] > FOAM FATAL ERROR: [5] Maximum number of iterations exceeded [5] [5] From function thermo<Thermo, Type>::T(scalar f, scalar T0, scalar (thermo<Thermo, Type>::*F)(const scalar) const, scalar (thermo<Thermo, Type>::*dFdT)(const scalar) const, scalar (thermo<Thermo, Type>::*limit)(const scalar) const) const [5] in file /home/shorty/OpenFOAM/OpenFOAM2.2.x/src/thermophysicalModels/specie/lnInclude/thermoI.H at line 76. [5] FOAM parallel run aborting [5] [5] #0 Foam::error::printStack(Foam::Ostream&) in "/home/shorty/OpenFOAM/OpenFOAM2.2.x/platforms/linux64Gcc47DPOpt/lib/libOpenFOAM.so" [5] #1 Foam::error::abort() in "/home/shorty/OpenFOAM/OpenFOAM2.2.x/platforms/linux64Gcc47DPOpt/lib/libOpenFOAM.so" [5] #2 Foam::species::thermo<Foam::hPolynomialThermo<Foam::icoPolynomial<Foam::specie, 8>, 8>, Foam::sensibleEnthalpy>::T(double, double, double, double (Foam::species::thermo<Foam::hPolynomialThermo<Foam::icoPolynomial<Foam::specie, 8>, 8>, Foam::sensibleEnthalpy>::*)(double, double) const, double (Foam::species::thermo<Foam::hPolynomialThermo<Foam::icoPolynomial<Foam::specie, 8>, 8>, Foam::sensibleEnthalpy>::*)(double, double) const, double (Foam::species::thermo<Foam::hPolynomialThermo<Foam::icoPolynomial<Foam::specie, 8>, 8>, Foam::sensibleEnthalpy>::*)(double) const) const in "/home/shorty/OpenFOAM/OpenFOAM2.2.x/platforms/linux64Gcc47DPOpt/lib/libfluidThermophysicalModels.so" [5] #3 Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::polynomialTransport<Foam::species::thermo<Foam::hPolynomialThermo<Foam::icoPolynomial<Foam::specie, 8>, 8>, Foam::sensibleEnthalpy>, 8> > >::calculate() in "/home/shorty/OpenFOAM/OpenFOAM2.2.x/platforms/linux64Gcc47DPOpt/lib/libfluidThermophysicalModels.so" [5] #4 Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::polynomialTransport<Foam::species::thermo<Foam::hPolynomialThermo<Foam::icoPolynomial<Foam::specie, 8>, 8>, Foam::sensibleEnthalpy>, 8> > >::correct() in "/home/shorty/OpenFOAM/OpenFOAM2.2.x/platforms/linux64Gcc47DPOpt/lib/libfluidThermophysicalModels.so" [5] #5 [5] in "/home/shorty/OpenFOAM/OpenFOAM2.2.x/platforms/linux64Gcc47DPOpt/bin/buoyantSimpleFoam" [5] #6 __libc_start_main in "/lib/x86_64linuxgnu/libc.so.6" [5] #7 [5] in "/home/shorty/OpenFOAM/OpenFOAM2.2.x/platforms/linux64Gcc47DPOpt/bin/buoyantSimpleFoam" Code:
p0 = p_rgh + rho*gh Because my tank is 2m high and the fluid is water (1000kg/m³). So as I see in this formula the higher I get in the tank the lower p0 should be because: Code:
rho ~ 1000kg/m³ g = 9,81 h raises p0 = p_rgh  1000* 9,81 * 2 Therefor p and p_rgh should not be the same? 

October 31, 2013, 06:08 

#6 
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Tussenhausen
Posts: 2,679
Blog Entries: 6
Rep Power: 49 
Hi all,
just one question. Why is in interFoam the p0 calculation for nonclosedVolumes like that: Code:
p == p_rgh + rho*gh; Code:
p = p_rgh + rho*gh; Tobi 

October 31, 2013, 14:56 

#7 
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Tussenhausen
Posts: 2,679
Blog Entries: 6
Rep Power: 49 
Hi all,
I made a test with chtMultiRegionSimpleFoam with only one region. Just a very simple case  box with inlet and outlet at the top of the box. If I use the thermodynamics out of the liquidHeater tutorial: Code:
thermoType { type heRhoThermo; mixture pureMixture; transport const; thermo hConst; equationOfState rhoConst; specie specie; energy sensibleEnthalpy; } mixture { specie { nMoles 1; molWeight 18; } equationOfState { rho 1000; } thermodynamics { Cp 4181; Hf 0; } transport { mu 959e6; Pr 6.62; } } After switching to my own thermodynamic with the polynoms its blow up after the 4th iteration: Code:
thermoType { type heRhoThermo; mixture pureMixture; transport polynomial; thermo hPolynomial; equationOfState icoPolynomial; specie specie; energy sensibleEnthalpy; } mixture { specie { nMoles 1; molWeight 18; } equationOfState { rhoCoeffs<8> (611.705 2.78 0.005 5.58512e13 4.3231e16 0 0 0); } thermodynamics { Hf 0; Sf 0; CpCoeffs<8> (5158.69 6.26 0.01 6.17887e12 4.78243e15 0 0 0); } transport { muCoeffs<8> (0.000292721 3.33273e6 1.43625e8 2.76923e11 2.0125e14 0 0 0); kappaCoeffs<8> (55.2758 0.683843 0.00315152 6.47667e6 5e9 0 0 0); } } Therefor I made a test just with the first coefficient like: Code:
rhoCoeffs<8> (1000 0 0 0 0 0 0 0); Code:
> FOAM FATAL ERROR: Maximum number of iterations exceeded From function thermo<Thermo, Type>::T(scalar f, scalar T0, scalar (thermo<Thermo, Type>::*F)(const scalar) const, scalar (thermo<Thermo, Type>::*dFdT)(const scalar) const, scalar (thermo<Thermo, Type>::*limit)(const scalar) const) const in file /home/shorty/OpenFOAM/OpenFOAM2.2.x/src/thermophysicalModels/specie/lnInclude/thermoI.H at line 76. FOAM aborting #0 Foam::error::printStack(Foam::Ostream&) in "/home/shorty/OpenFOAM/OpenFOAM2.2.x/platforms/linux64Gcc47DPOpt/lib/libOpenFOAM.so" #1 Foam::error::abort() in "/home/shorty/OpenFOAM/OpenFOAM2.2.x/platforms/linux64Gcc47DPOpt/lib/libOpenFOAM.so" #2 Foam::species::thermo<Foam::hPolynomialThermo<Foam::icoPolynomial<Foam::specie, 8>, 8>, Foam::sensibleEnthalpy>::T(double, double, double, double (Foam::species::thermo<Foam::hPolynomialThermo<Foam::icoPolynomial<Foam::specie, 8>, 8>, Foam::sensibleEnthalpy>::*)(double, double) const, double (Foam::species::thermo<Foam::hPolynomialThermo<Foam::icoPolynomial<Foam::specie, 8>, 8>, Foam::sensibleEnthalpy>::*)(double, double) const, double (Foam::species::thermo<Foam::hPolynomialThermo<Foam::icoPolynomial<Foam::specie, 8>, 8>, Foam::sensibleEnthalpy>::*)(double) const) const in "/home/shorty/OpenFOAM/OpenFOAM2.2.x/platforms/linux64Gcc47DPOpt/lib/libfluidThermophysicalModels.so" #3 Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::polynomialTransport<Foam::species::thermo<Foam::hPolynomialThermo<Foam::icoPolynomial<Foam::specie, 8>, 8>, Foam::sensibleEnthalpy>, 8> > >::calculate() in "/home/shorty/OpenFOAM/OpenFOAM2.2.x/platforms/linux64Gcc47DPOpt/lib/libfluidThermophysicalModels.so" #4 Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::polynomialTransport<Foam::species::thermo<Foam::hPolynomialThermo<Foam::icoPolynomial<Foam::specie, 8>, 8>, Foam::sensibleEnthalpy>, 8> > >::correct() in "/home/shorty/OpenFOAM/OpenFOAM2.2.x/platforms/linux64Gcc47DPOpt/lib/libfluidThermophysicalModels.so" #5 in "/home/shorty/OpenFOAM/OpenFOAM2.2.x/platforms/linux64Gcc47DPOpt/bin/chtMultiRegionSimpleFoam" #6 __libc_start_main in "/lib/x86_64linuxgnu/libc.so.6" #7 in "/home/shorty/OpenFOAM/OpenFOAM2.2.x/platforms/linux64Gcc47DPOpt/bin/chtMultiRegionSimpleFoam" Abgebrochen (Speicherabzug geschrieben) I am out of mind and have no further ideas at the moment. Regards Tobi 

October 31, 2013, 15:12 

#8 
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Tussenhausen
Posts: 2,679
Blog Entries: 6
Rep Power: 49 
Hi all,
just notice: I am stupid! All values of mu are wrong. Instead of writing: 503,89e6 I wrote 0,50389e6 After changing this, the easy test case is working. Now I am going to check if my bigger project is working too. 

October 31, 2013, 17:10 

#9 
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Tussenhausen
Posts: 2,679
Blog Entries: 6
Rep Power: 49 
Okay.
I checked it out with the other case. Without gravity its working (bouyantSimpleFoam and chtMultiRegionSimpleFoam). But after switching on the gravity its still the same. Regards Tobi 

October 31, 2013, 21:28 

#10 
Senior Member
Joachim Herb
Join Date: Sep 2010
Posts: 649
Rep Power: 20 
Perhaps your problem is the same as described in this thread:
http://www.cfdonline.com/Forums/ope...roperties.html You could also try the transient solver (buoyantPimpleFoam) 

November 4, 2013, 05:03 

#11 
Member
hannes
Join Date: Mar 2013
Posts: 47
Rep Power: 11 
Dear Tobi,
the pictures you showed match exactly the problem we had. I'm pretty sure that your results will improve when you start the simulations with hydrostatic pressure distribution for p. What happens is when you turn on gravity the pressure field rapidly changes in order to be consistent so that's why you get those strong gradients in the p_rgh field which again results in the high velocities. If you don't want to set your p field with funkySetFields then you should adapt your solver. Copy the solver and the only thing you have to change in createFields.H is the line reading Code:
p_rgh = p  rho*gh; Replace it by solving for p: Code:
p = p_rgh + rho*gh Regards Hannes 

November 4, 2013, 07:43 

#12 
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Tussenhausen
Posts: 2,679
Blog Entries: 6
Rep Power: 49 
Hi all,
thanks for the hints but it is still not working. On my easy case the chtMultiRegionSimpleFoam solver (only with one domain) is working. But the buoyantSimpleFoam is not working. Additionally I tryed the hints hannes said but not with success. In the attachment you find a picture of the chtMultiSImpleFoam solver and the solution. I have no further idea at the moment. For me it seems that the buoyantSimpleFoam is not a good solver for the thing I want to do. Furthermore the chtMultiSimpleFoam solver is not working in my big case too. Thanks for your help but I think I have to give up on that project. Maybe "WATER" is not very common for the solvers. At least I had a look into the cht solver and the createFields.H file. There is the same calculation as in the buoyantSimpleFoam. So I have no idea why this solver is working and the other one not :/ Regards Tobi 

November 4, 2013, 08:26 

#13 
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Tussenhausen
Posts: 2,679
Blog Entries: 6
Rep Power: 49 
Hi all,
now the pressure fields are the same (buoyantSimpleFoam and chtMultiRegionSimpleFoam) . I had to change the schemes to get the same results Now I am going to check if its working wit a bigger domain. 

November 4, 2013, 09:50 

#14 
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Tussenhausen
Posts: 2,679
Blog Entries: 6
Rep Power: 49 
Summary with a bigger domain:
 chtMultiRegionSimpleFoam isn 't working anymore  buoyantSimpleFoam isn 't working anymore  myBuoyantSimpleFoam with the modification in the createFields.H is working. Hannes I think the work is done now. I will check my official geometry now. I keep you posted. 

November 4, 2013, 10:26 

#15  
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Tussenhausen
Posts: 2,679
Blog Entries: 6
Rep Power: 49 
Quote:
Thanks a lot. Just one question to that. Why isn 't it implemented as you wrote? I think there is any reason for that? Additionally with the PIMPLE algorithm it is not working. Do you have any experience with that? Maybe I will initialize it with simple and then switch to pimple. Regards Tobi Last edited by Tobi; November 4, 2013 at 11:35. 

November 5, 2013, 13:25 

#16 
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Tussenhausen
Posts: 2,679
Blog Entries: 6
Rep Power: 49 
Hi all,
with the modified buoyantSimpleFoam solver my case is working and the steady state result is very nice. After initialize this solution with the buoyantPimpleFoam solver I get crazy p_rgh and p fields again 

November 6, 2013, 10:53 

#17 
Member
hannes
Join Date: Mar 2013
Posts: 47
Rep Power: 11 
Hi Tobi,
I can't really tell you why it is implemented that way, I'm not aware of any restrictions at that point. Maybe the thinking is, that it is easier to initialise a pressure field which is a little more intuitiv then to initialise p_rgh when not starting with constant fields. However, concerning the problem with buoyantPimpleFoam I could only guess. First of all, one thing that might become neccessary is to increase your writePrecision in controlDict, the standard six (or eight?) digits are by far not sufficient when small fluctuations in p_rgh are concerned, so that might be a reason why a restart might fail. Otherwise it should be possible to run the simulation with the buoyantPimpleFoam starting from a constant field when the same change to the solver is performed (change in createFields.H). Could you provide some more information on the crash if the above does not help? Hannes 

November 6, 2013, 12:03 

#18 
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Tussenhausen
Posts: 2,679
Blog Entries: 6
Rep Power: 49 
Dear Hannes,
thanks for your replay. I also tried to start the simulation with the change in the createField.H. But without success. Additionally I changed the time precision like you said but the same  crash. Here is the output: Code:
Starting time loop Courant Number mean: 6.92740210013e09 max: 4.85034908134e06 deltaT = 1.199999616e07 Time = 1.2e07 diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 DILUPBiCG: Solving for Ux, Initial residual = 2.28465064941e09, Final residual = 2.28465064941e09, No Iterations 0 DILUPBiCG: Solving for Uy, Initial residual = 2.43944451461e09, Final residual = 2.43944451461e09, No Iterations 0 DILUPBiCG: Solving for Uz, Initial residual = 1.09072719922e09, Final residual = 1.09072719922e09, No Iterations 0 DILUPBiCG: Solving for h, Initial residual = 3.35094034737e06, Final residual = 2.93432135474e18, No Iterations 1 GAMG: Solving for p_rgh, Initial residual = 0.999966166727, Final residual = 4.61953060743e07, No Iterations 25 diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 time step continuity errors : sum local = 7.21330773016e17, global = 3.97805509428e17, cumulative = 3.97805509428e17 ExecutionTime = 42.62 s ClockTime = 60 s Courant Number mean: 8.31290630685e09 max: 5.82512408095e06 deltaT = 1.43999933184e07 Time = 2.64e07 diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 DILUPBiCG: Solving for Ux, Initial residual = 0.000359951353176, Final residual = 2.99850393754e17, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 0.000406515147044, Final residual = 4.7022285039e17, No Iterations 1 DILUPBiCG: Solving for Uz, Initial residual = 5.62159242983e05, Final residual = 3.53128489406e18, No Iterations 1 DILUPBiCG: Solving for h, Initial residual = 0.000118849971877, Final residual = 8.30419637485e17, No Iterations 1 GAMG: Solving for p_rgh, Initial residual = 0.503136149457, Final residual = 2.61630245853e07, No Iterations 26 diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 time step continuity errors : sum local = 3.97094383529e17, global = 1.86616925674e17, cumulative = 5.84422435102e17 ExecutionTime = 66.02 s ClockTime = 89 s Courant Number mean: 9.97543173077e09 max: 6.99668194517e06 deltaT = 1.72799880008e07 Time = 4.368e07 diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 DILUPBiCG: Solving for Ux, Initial residual = 0.00020724814406, Final residual = 5.63890977966e17, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 0.000235776423607, Final residual = 4.17515596363e17, No Iterations 1 DILUPBiCG: Solving for Uz, Initial residual = 3.23259354164e05, Final residual = 1.41492437006e17, No Iterations 1 DILUPBiCG: Solving for h, Initial residual = 0.999999131419, Final residual = 1.4011399717e14, No Iterations 1 GAMG: Solving for p_rgh, Initial residual = 0.999982729227, Final residual = 9.81585468245e07, No Iterations 52 diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 time step continuity errors : sum local = 1.90312676653e13, global = 1.04003980939e14, cumulative = 1.03419558504e14 ExecutionTime = 100.86 s ClockTime = 130 s Courant Number mean: 0.00016710031461 max: 0.221478550247 deltaT = 3.90105209282e08 Time = 4.7581e07 diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 DILUPBiCG: Solving for Ux, Initial residual = 0.0892826131216, Final residual = 3.47960960238e10, No Iterations 2 DILUPBiCG: Solving for Uy, Initial residual = 0.0860767448894, Final residual = 2.07507793124e10, No Iterations 2 DILUPBiCG: Solving for Uz, Initial residual = 0.00526497170747, Final residual = 5.00604327108e07, No Iterations 1 DILUPBiCG: Solving for h, Initial residual = 0.999999999974, Final residual = 1.22827994334e07, No Iterations 1 #0 Foam::error::printStack(Foam::Ostream&) in "/home/shorty/OpenFOAM/OpenFOAM2.2.x/platforms/linux64Gcc47DPOpt/lib/libOpenFOAM.so" #1 Foam::sigFpe::sigHandler(int) in "/home/shorty/OpenFOAM/OpenFOAM2.2.x/platforms/linux64Gcc47DPOpt/lib/libOpenFOAM.so" #2 in "/lib/x86_64linuxgnu/libc.so.6" #3 Foam::GAMGSolver::scale(Foam::Field<double>&, Foam::Field<double>&, Foam::lduMatrix const&, Foam::FieldField<Foam::Field, double> const&, Foam::UPtrList<Foam::lduInterfaceField const> const&, Foam::Field<double> const&, unsigned char) const in "/home/shorty/OpenFOAM/OpenFOAM2.2.x/platforms/linux64Gcc47DPOpt/lib/libOpenFOAM.so" #4 Foam::GAMGSolver::Vcycle(Foam::PtrList<Foam::lduMatrix::smoother> const&, Foam::Field<double>&, Foam::Field<double> const&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::PtrList<Foam::Field<double> >&, Foam::PtrList<Foam::Field<double> >&, unsigned char) const in "/home/shorty/OpenFOAM/OpenFOAM2.2.x/platforms/linux64Gcc47DPOpt/lib/libOpenFOAM.so" #5 Foam::GAMGSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/home/shorty/OpenFOAM/OpenFOAM2.2.x/platforms/linux64Gcc47DPOpt/lib/libOpenFOAM.so" #6 Foam::fvMatrix<double>::solveSegregated(Foam::dictionary const&) in "/home/shorty/OpenFOAM/OpenFOAM2.2.x/platforms/linux64Gcc47DPOpt/lib/libfiniteVolume.so" #7 Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/home/shorty/OpenFOAM/shorty2.2.x/platforms/linux64Gcc47DPOpt/bin/myBuoyantPimpleFoam" #8 in "/home/shorty/OpenFOAM/shorty2.2.x/platforms/linux64Gcc47DPOpt/bin/myBuoyantPimpleFoam" #9 __libc_start_main in "/lib/x86_64linuxgnu/libc.so.6" #10 in "/home/shorty/OpenFOAM/shorty2.2.x/platforms/linux64Gcc47DPOpt/bin/myBuoyantPimpleFoam" GleitkommaAusnahme (Speicherabzug geschrieben) Regards Tobi 

November 6, 2013, 12:32 

#19 
Senior Member
Joachim Herb
Join Date: Sep 2010
Posts: 649
Rep Power: 20 
If I read your log file correctly, you don't use the nOuterCorrectors loop. Have you tried nOuterCorrectors > 1 with underrelaxation?


November 6, 2013, 18:34 

#20 
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Tussenhausen
Posts: 2,679
Blog Entries: 6
Rep Power: 49 
Hi,
PIMPLE and underrelaxation? Is underrelaxation not changing the real solution (accuracy in time)? Well I used nOuterCorrectors > 1 but without success anyway. The error is different. I reach the maximum iteration in the temperature calculation: Code:
Courant Number mean: 6.92740210013e09 max: 4.85034908134e06 deltaT = 1.199999616e07 Time = 1.2e07 diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 PIMPLE: iteration 1 DILUPBiCG: Solving for Ux, Initial residual = 4.38718521517e07, Final residual = 4.38718521517e07, No Iterations 0 DILUPBiCG: Solving for Uy, Initial residual = 4.74501872065e07, Final residual = 4.74501872065e07, No Iterations 0 DILUPBiCG: Solving for Uz, Initial residual = 1.12086811751e07, Final residual = 1.12086811751e07, No Iterations 0 DILUPBiCG: Solving for h, Initial residual = 3.35094034737e06, Final residual = 2.93432135474e18, No Iterations 1 GAMG: Solving for p_rgh, Initial residual = 0.997921524511, Final residual = 0.00514407773528, No Iterations 3 diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 time step continuity errors : sum local = 1.62324329599e14, global = 2.43019772121e17, cumulative = 2.43019772121e17 PIMPLE: iteration 2 DILUPBiCG: Solving for Ux, Initial residual = 8.49053274605e06, Final residual = 1.56889161256e18, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 9.2706169794e06, Final residual = 1.7128784731e18, No Iterations 1 DILUPBiCG: Solving for Uz, Initial residual = 2.42439406856e06, Final residual = 6.15472389836e19, No Iterations 1 DILUPBiCG: Solving for h, Initial residual = 9.4741734031e05, Final residual = 4.43794077117e17, No Iterations 1 GAMG: Solving for p_rgh, Initial residual = 0.19770073244, Final residual = 0.00135321069298, No Iterations 3 diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 time step continuity errors : sum local = 7.92499613563e15, global = 2.83812616391e17, cumulative = 4.07928442704e18 PIMPLE: iteration 3 DILUPBiCG: Solving for Ux, Initial residual = 5.83420314596e06, Final residual = 9.42862909442e19, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 6.40245339442e06, Final residual = 1.01498615559e18, No Iterations 1 DILUPBiCG: Solving for Uz, Initial residual = 1.25166849944e06, Final residual = 2.97094658592e19, No Iterations 1 DILUPBiCG: Solving for h, Initial residual = 0.999998344609, Final residual = 1.3555675042e14, No Iterations 1 GAMG: Solving for p_rgh, Initial residual = 0.999975236161, Final residual = 9.72118583228e07, No Iterations 53 diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 time step continuity errors : sum local = 9.88922463867e14, global = 5.09467127861e15, cumulative = 5.09875056304e15 ExecutionTime = 55.77 s ClockTime = 56 s Courant Number mean: 8.77396468445e05 max: 0.116223720973 deltaT = 5.162455599e08 Time = 1.71625e07 diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 PIMPLE: iteration 1 DILUPBiCG: Solving for Ux, Initial residual = 0.157070886327, Final residual = 5.76405070912e06, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 0.150534403994, Final residual = 6.62063104725e06, No Iterations 1 DILUPBiCG: Solving for Uz, Initial residual = 0.0099884610888, Final residual = 9.50614332261e07, No Iterations 1 DILUPBiCG: Solving for h, Initial residual = 0.999999999998, Final residual = 1.22959247587e07, No Iterations 1 GAMG: Solving for p_rgh, Initial residual = 0.999999956955, Final residual = 0.00978329204882, No Iterations 132 diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 time step continuity errors : sum local = 0.00980931633566, global = 1.15347141494e05, cumulative = 1.15347141443e05 PIMPLE: iteration 2 DILUPBiCG: Solving for Ux, Initial residual = 0.999932390446, Final residual = 0.0990621421236, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 0.999999756929, Final residual = 0.0923265680759, No Iterations 1 DILUPBiCG: Solving for Uz, Initial residual = 0.998134013837, Final residual = 0.046339171224, No Iterations 3 DILUPBiCG: Solving for h, Initial residual = 1, Final residual = 0.0804871336416, No Iterations 25 > FOAM FATAL ERROR: Maximum number of iterations exceeded From function thermo<Thermo, Type>::T(scalar f, scalar T0, scalar (thermo<Thermo, Type>::*F)(const scalar) const, scalar (thermo<Thermo, Type>::*dFdT)(const scalar) const, scalar (thermo<Thermo, Type>::*limit)(const scalar) const) const in file /home/shorty/OpenFOAM/OpenFOAM2.2.x/src/thermophysicalModels/specie/lnInclude/thermoI.H at line 76. FOAM aborting #0 Foam::error::printStack(Foam::Ostream&) in "/home/shorty/OpenFOAM/OpenFOAM2.2.x/platforms/linux64Gcc47DPOpt/lib/libOpenFOAM.so" #1 Foam::error::abort() in "/home/shorty/OpenFOAM/OpenFOAM2.2.x/platforms/linux64Gcc47DPOpt/lib/libOpenFOAM.so" #2 Foam::species::thermo<Foam::hPolynomialThermo<Foam::icoPolynomial<Foam::specie, 8>, 8>, Foam::sensibleEnthalpy>::T(double, double, double, double (Foam::species::thermo<Foam::hPolynomialThermo<Foam::icoPolynomial<Foam::specie, 8>, 8>, Foam::sensibleEnthalpy>::*)(double, double) const, double (Foam::species::thermo<Foam::hPolynomialThermo<Foam::icoPolynomial<Foam::specie, 8>, 8>, Foam::sensibleEnthalpy>::*)(double, double) const, double (Foam::species::thermo<Foam::hPolynomialThermo<Foam::icoPolynomial<Foam::specie, 8>, 8>, Foam::sensibleEnthalpy>::*)(double) const) const in "/home/shorty/OpenFOAM/OpenFOAM2.2.x/platforms/linux64Gcc47DPOpt/lib/libfluidThermophysicalModels.so" #3 Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::polynomialTransport<Foam::species::thermo<Foam::hPolynomialThermo<Foam::icoPolynomial<Foam::specie, 8>, 8>, Foam::sensibleEnthalpy>, 8> > >::calculate() in "/home/shorty/OpenFOAM/OpenFOAM2.2.x/platforms/linux64Gcc47DPOpt/lib/libfluidThermophysicalModels.so" #4 Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::polynomialTransport<Foam::species::thermo<Foam::hPolynomialThermo<Foam::icoPolynomial<Foam::specie, 8>, 8>, Foam::sensibleEnthalpy>, 8> > >::correct() in "/home/shorty/OpenFOAM/OpenFOAM2.2.x/platforms/linux64Gcc47DPOpt/lib/libfluidThermophysicalModels.so" #5 in "/home/shorty/OpenFOAM/OpenFOAM2.2.x/platforms/linux64Gcc47DPOpt/bin/buoyantPimpleFoam" #6 __libc_start_main in "/lib/x86_64linuxgnu/libc.so.6" #7 in "/home/shorty/OpenFOAM/OpenFOAM2.2.x/platforms/linux64Gcc47DPOpt/bin/buoyantPimpleFoam" Abgebrochen (Speicherabzug geschrieben) 

Thread Tools  Search this Thread 
Display Modes  

