[melanie]

thanks Gavin, indeed my rho field is not intialized anywhere and I guess it takes 0.
I looked into the coodles tutorial, and there is either no rho file in the constant/0 directory, rho is just created at the first time step.
Should I create a rho file with a standard value ?
mélanie

[gschaider]

@melanies nan-Courant's: That's just a guess: I think I had similar problems with other solvers where adjustTimeStep was yes and maxDeltaT was 0 (which of course doesn't make too much sense, but there are cases floating around where it's set that way).

[melanie]

I think I have found something: in incompressible solvers (my initial condition is incompressible), p is calculated from p/rho with reference 0 Pa in my case. It means that my initial pressure field is not absolute, but relative to p_ref. I changed the value of p_ref to 101300 Pa, but no change, I get the same error.
mélanie

[grtabor]

>thanks Gavin, indeed my rho field is not intialized anywhere and I guess it takes 0.
>I looked into the coodles tutorial, and there is either no rho file in the constant/0 directory, rho is just created at the first time step.
>Should I create a rho file with a standard value ?
>mélanie

I'd try that as a first guess, although its been a while since I last ran coodles (8 years?)

Gavin

[eugene]

Things you should do before running coodles:
1. Change the p dimensions from [0 2 -2 0 0 0 0] to [1 -1 -2 0 0 0 0].
2. Change the new p to absolute values
3. Delete phi and phi_0
4. Coodles uses the thermo package to calculate rho. So you need the right entries in your thermophysicalProperties dictionary.
5. Make the outlet pressure boundary non-reflecting (otherwise you will get waves bouncing up and down your domain).
6. Change nuSgs to muSgs. Also modify the units.
7. Use the fvScemes, fvSolotion and controlDict from the coodles tutorial.

Thats all I can think of for now, but there is probably some things I have missed.

[melanie]

Eugene, that's what I did:

1. already done,
2. I changed with no more results,
3. actually there was no phi* file,
4. basic flow, identical to coodles tutorial,
5. what is the name of this pressure non-reflective BC? and what are the conditions on the fields ?
6. already done,
7. already done.

Bernhard: my timestep is fixed, no such problems.

[eugene]

"pressureTransmissive" is the BC name.
I think it takes a Linf (wave length scale - don't ask), Pinf (target pressure) and a value entry.

Checking your error post again, my best guess is that either your temperature or pressure field is broken. For "nan" to come up before you have even started solving means you probably have either p=0 or T=0 somewhere in your initial fields. If you stick either of these into the thermo package it will give you bollocks. You need physically realistic values for temperature and pressure for coodles to work.

Add the following lines to your code before the Ueqn.H entry:

Info<< "rho max/min : " << gMax(rho) << " " << gMin(rho) << endl;
Info<< "p max/min : " << gMax(p) << " " << gMin(p) << endl;

Should give you an idea of what is going wrong.

[melanie]

Thanks Eugene.
Firstly I foun errors in my initial temperature field; then I modified the source file like you sais to check max/min rho and p (OK), and I still got the same error message just before solving p (here follows the end of the log-file):

Starting time loop

Time = 1e-06

Mean and max Courant Numbers = 0.005518647 0.18159526
BICCG: Solving for Ux, Initial residual = 9.2946507e-05, Final residual = 4.9573551e-08, No Iterations 1
BICCG: Solving for Uy, Initial residual = 0.00016879922, Final residual = 7.0933073e-11, No Iterations 2
BICCG: Solving for h, Initial residual = 1, Final residual = 2.1862895e-10, No Iterations 3
rho max/min: 1.1827567 1.163765
p max/min: 102083.49 100442.93

Something may be wrong in the pressure field, but how to know where ?

[pierre]

How about initialising with rhoSimpleFoam?

Pierre

[melanie]

I just wanted to start from the same initial conditions, it is possible with Fluent to turn on the compressibility on the fly, why not with OpenFOAM ?
If I don't find the mistake, I know that this will be the thing to do...
mélanie

[mirsaeedi]

Hi
I solved a turbulent pipe flow with LES but results do not match with experimental datas!
can anyone help me?

[mirsaeedi]

Hi
I solved a turbulent pipe flow with LES but results do not match with experimental datas!
can anyone help me?

[mahaputra]

Dear Melanie


did you success to run your modified simpleFoam case on LES solver?

please let me know, since im facing similar problem.


could anybody kindly post here, how to solve the problem ?

i followed the tips from eugene , i tried to run 2d case on coodles, but its courant number becomes exploded in time 6 :


Time = 6

Courant Number mean: 17306 max: 1.00279e+07
diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
DILUPBiCG: Solving for Ux, Initial residual = 0.918686, Final residual = 4.97796, No Iterations 1001
DILUPBiCG: Solving for Uy, Initial residual = 0.833987, Final residual = 17.7067, No Iterations 1001
DILUPBiCG: Solving for h, Initial residual = 0.998159, Final residual = 0.267814, No Iterations 1001


Maximum number of iterations exceeded#0 Foam::error:rintStack(Foam::Ostream&) in "/home/user/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libOpenFOAM.so"
#1 Foam::error::abort() in "/home/user/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libOpenFOAM.so"
#2 Foam::hThermo<Foam:ureMixture<Foam::constTranspo rt<Foam::specieThermo<Foam::hConstThermo<Foam:er fectGas> > > > >::calculate() in "/home/user/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libbasicThermophysicalModels.so"
#3 Foam::hThermo<Foam:ureMixture<Foam::constTranspo rt<Foam::specieThermo<Foam::hConstThermo<Foam:er fectGas> > > > >::correct() in "/home/user/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libbasicThermophysicalModels.so"
#4 main in "/home/user/OpenFOAM/OpenFOAM-1.5/applications/bin/linuxGccDPOpt/coodles"
#5 __libc_start_main in "/lib/tls/i686/cmov/libc.so.6"
#6 Foam::regIOobject::readIfModified() in "/home/user/OpenFOAM/OpenFOAM-1.5/applications/bin/linuxGccDPOpt/coodles"


From function specieThermo<thermo>::T(scalar f, scalar T0, scalar (specieThermo<thermo>::*F)(const scalar) const, scalar (specieThermo<thermo>::*dFdT)(const scalar) const) const
in file /home/dm2/henry/OpenFOAM/OpenFOAM-1.5/src/thermophysicalModels/specie/lnInclude/specieThermoI.H at line 78.

FOAM aborting

[klilla]

Dear All,

I tried to simulate an acoustic pulse placed in the middle of a rectangular domain. The pulse should spread with the speed of sound unidirectionally. This happens well, BUT, in the density field there remains a smaller pulse constantly. This I do not understand, it seams that there and entropy pulse created, due to I do not know what.

My initial problem:

velocity is zero everywhere
gaussian pulse of pressure at the center of the domain (set by funkySet Field)
Op. 1: constant temperature, hoping that the "thermo" package will set the density well
Op. 2: set the density too as a gauss pressure rho = 1/(c*c)*p

Both initializations give back exactly the same results.

I normalized the pressure by pNorm = p/(c*c) +0.327 where the correction is exactly the same as the amplitude of the remaining pulse. In this case the density and normP plots are the same (except that in the density there is the extra bump )

have you any idea where I introduce this additional pulse?

Thanks,

Lilla