CFD Online Discussion Forums

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (https://www.cfd-online.com/Forums/openfoam-solving/)
-   -   reactingFoam with very high temperatures (https://www.cfd-online.com/Forums/openfoam-solving/167329-reactingfoam-very-high-temperatures.html)

liguobing00 February 28, 2016 08:50

reactingFoam with very high temperatures
 
1 Attachment(s)
Hello, every one!

First of all, I am new in OF, and I am not very good at English. This is my first time to asking on this website. Sorry about that.(and the title)
I have come to a problem lately when I solved a case using reactingFoam. the geometry is quite simple, just like a channel with premixed CH4 flows in and products flows out, there should have a flame attach to part of the wall with high temperature.

but I keep coming to an error, temperature very high and dt very short, so my program stuck and can not calculate any further.


the error:


--> FOAM Warning :
From function janafThermo<EquationOfState>::limit(const scalar T) const
in file /opt/OpenFOAM/OpenFOAM-2.3.1/src/thermophysicalModels/specie/lnInclude/janafThermoI.H at line 108
attempt to use janafThermo<EquationOfState> out of temperature range 200 -> 5000; T = 5782.25
--> FOAM Warning :
From function janafThermo<EquationOfState>::limit(const scalar T) const
in file /opt/OpenFOAM/OpenFOAM-2.3.1/src/thermophysicalModels/specie/lnInclude/janafThermoI.H at line 108
attempt to use janafThermo<EquationOfState> out of temperature range 200 -> 5000; T = 5780.25
--> FOAM Warning :
From function janafThermo<EquationOfState>::limit(const scalar T) const
in file /opt/OpenFOAM/OpenFOAM-2.3.1/src/thermophysicalModels/specie/lnInclude/janafThermoI.H at line 108
attempt to use janafThermo<EquationOfState> out of temperature range 200 -> 5000; T = 5768.95
--> FOAM Warning :


Swagga5aur June 8, 2017 10:31

Hello liguobing,
I have taken a look at your files and modified them to get a solution and I will attach the changed files for you when I'm done, note that I use OF4.1.

In the following a brief explanation of the changes I currently have made are given:

First of all the specified mass fractions results in a summation above 1, which is should be equal to 1 at all times, due to this, I altered the mass fractions of the H2O and CH4 at the inlet.

The outlet of the combustion chamber was altered for the different boundary conditions such as T being specified to be a fixedValue, changed this to an inletOutlet boundary condition instead.

Additionally, note that you specified the hot plate temperature of 800 only at the bot patch, I don't know if its supposed to be so, so I applied to 800K at the four hot patches.

I'll get back to you as soon as possible, when I have tested the case more thoroughly.

Swagga5aur June 10, 2017 17:35

1 Attachment(s)
I have now determined the issue besides the previous post changes. With the specified geometry and flow velocities the resulting contracted flow in the heating pipe is turbulent making a laminar combustion model inadequate. Additionally, to capture the combustion process an increased mesh density was implemented in the domain.

I decreased the geometry size to secure laminar flow/combustion and attached the altered case to this post, however, if you wish to solve the original geometry and flow velocities the combustion model should be changed to possibly PaSR and the mesh density should be further increased, with an emphasis on the combustion zone.

Hope its of any help.


All times are GMT -4. The time now is 22:34.