View source for Talk:Tut reactingFoam firstTutorial

== adaption to OpenFOAM-1.6 ==

It is possible to use the tutorial in OpenFOAM-1.6 with some minor changes:

* a "g"-file is needed in the /constant directory, which can be used from the new aachenBomb-tutorial
* file "constant/chemistryProperties" 
** <code>chemistrySolver</code> should be <code>ode</code> instead of <code>ODE</code>
** there should be a <code>odeCoeffs</code>-dictionary instead of <code>ODECoeffs</code>
** added the line <code>psyChemistryModel ODEChemistryModel<gasThermoPhysics>;</code> after the header
* file "constant/thermophysicalProperties"
** replace line <code>thermoType hMixtureThermo<reactingMixture>;</code> by <code>thermoType hPsiMixtureThermo<reactingMixture<gasThermoPhysics>>;</code>
** check for correct places of CHEMKINFile and CHEMKINThermoFile, it works with <code>CHEMKINFile "../chemkin/chem.inp";</code> and <code>CHEMKINThermoFile "../chemkin/therm.dat";</code>
* file "0/T"
** in boundary condition "outlet", replace <code>type fixedValue; value uniform 800;</code> with <code>type zeroGradient;</code>
* a "constant/RASProperties"-file could be needed, examples can be found e.g. in the new aachenBomb-tutorial


--[[User:Aortwein|Aortwein]] 14:01, 12 May 2010 (UTC)

Now: adaptation to OpenFOAM-1.7.1 --[[User:Aortwein|Aortwein]] 13:23, 14 December 2010 (CET)

== older question ==

Thanks for the tutorial, however, I am getting the following error in the third time step, and have not been able to find the problem: 

--> FOAM FATAL ERROR : attempt to use janafThermo<equationOfState> out of temperature range 200 -> 5000;  T = 5000.92#0 

Any suggestions or a fix would be very appreciated.  Thanks again.  ~E
* a possibility could be to change the oxygen in the lowerInlet (in the the 0/O2 file) from 1.0 to (say) 0.9 or less and the nitrogen in the lowerInlet ( 0/N2) from 0.0 to 0.1 to cool down the reaction
* note: my suggestion is not validated, since I did not have that problem yet, but the problem is also discussed here: [http://www.cfd-online.com/Forums/openfoam-solving/57945-reactingfoam-2.html at cfd-online.com] --[[User:Aortwein|Aortwein]] 15:29, 4 December 2009 (UTC)
* as far as I can see, the main problem lies in the "T" file in the "0"-Directory. Here, the boundary condition for "outlet" is set to "type fixedValue" with a value of 800. That should be changed to "type zeroGradient", afterwards it should work. If that change is not done, obviously that boundary condition is making problems as soon as a temperature higher than 800 K reaches the outlet. --[[User:Aortwein|Aortwein]] 10:31, 16 December 2009 (UTC)
* One suggestion is to increase upper limit of the temperature in thermo.dat file. I have fixed this problem using this technique.