[hannes]

Hello everybody,

I am setting up an OpenFOAM computation with Xoodles. The problem consists of a swirling jet of premixed fuel/air that leaves a nozzle and hits a little cylinder that acts as a flame holder. The jet is surrounded by air.

I started by creating the model an using the thermophysicalProperties and combustionProperties from the Xoodles/pitzDaily tutorial.

Because of the inhomogeneous fuel distribution between jet and surrounding air I changed from homogeneousMixture to inhomogeneousMixture and set up a field "ft" with boundary conditions ft=0.6 in the nozzle and ft=0 elsewhere:

thermoType hhuMixtureThermo<inhomogeneousmixture<sutherlandtr ansport<speciethermo<janafther mo<perfectgas>>>>>;

I ran the case without igniting it and expected only mixing between jet and surrounding air.
But I found that the temperature in the mixing zone changed, even though I specified T=293K as initial Value for T and Tu inside the fields and on all boundaries. Finally the simulation stopped with the message:

--> FOAM FATAL ERROR : attempt to use janafThermo<equationofstate> out of temperature range 200 -> 5000; T = 196.182

From function janafThermo<equationofstate>::checkT(const scalar T) const
in file /home/dm2/henry/OpenFOAM/OpenFOAM-1.2/src/thermophysicalModels/specie/lnInclude/ janafThermoI.H at line 73.

It is not clear to me, where this temperature change comes from. Does anyone have an idea?

Thanks in advance,
Hannes

[niklas]

Are you using multivariate discretization?

N

[hannes]

Yes, I use the following configuration in fvSchemes:

div(phi,ft_b_h_hu) Gauss multivariateSelection
{
fu limitedLinear01 1;
ft limitedLinear01 1;
b limitedLinear01 1;
h limitedLinear 1;
hu limitedLinear 1;
};

[thumthae]

I think this error is a bug of combustion solver. This error I ever ask Mr.Henry in this Forum --> " http://www.cfd-online.com/OpenFOAM_D...tml?1117696728 "

on Friday, March 18, 2005

Henry found this is the problem with the heat transfer when you used hhu* thermodynamics packages like Xoodles, XiFoam and engineFoam and only for cases with fixed temperature walls.

So try to change wall boundary condition to adiabatic wall

Torn

[hannes]

Hello Chalothon,

thank you for your help. But I already read your discussion on this theme a while ago and had the same idea as you.
So I changed the boundary conditions to adiabatic walls (zero temperature gradient), but this did not change anything and the problem persists.

I have to mention, that I used the Xoodles/pitzDaily tutorial (2D) for this test, because it runs a lot faster than my case. When I change from homogeneousMixture to inhomogeneousMixture and specify "ft" at the inlet to something greater than zero, I also observe this temperature change.

Hannes

[hannes]

Now I changed to species with constant properties:
thermoType hhuMixtureThermo<inhomogeneousmixture<consttranspo rt<speciethermo<hconstthermo<p erfectgas>>>>>;

After looking into the code, I see that the enthalpy field is initialised to cp*T+Hf. When I change the heat of fusion Hf such, that both of the mixing species have the same enthalpy at the prescribed uniform temperature, i.e. the enthalpy field is initially uniform, then the temperature remains uniform while the species mix.
Does this mean that there is an inconsistency between species transport and enthalpy transport?