CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   Xoodles PitzDaily out of temperature rangepersisten error (http://www.cfd-online.com/Forums/openfoam-solving/59505-xoodles-pitzdaily-out-temperature-rangepersisten-error.html)

arkangel April 10, 2007 05:56

Hi in a domain of the scale fo
 
Hi in a domain of the scale found in pitzDaily, What are the parameters to be chosen in ignites sites in order to ensure a complete combustion.

All is running stable and then an error
FOAM FATAL ERROR : attempt to use janafThermo<equationofstate> out of temperature range 200 -> 6000;

I saw a lot of people having this error , so far noone has a satisfactory answer

the Courant number is normally less than 1.5
and b -min(b)- is bound to be close to 0 (O(e-12)) with a combustion progress of 50 or 60 %

What else can be wrong

arkangel April 11, 2007 05:05

No one?
 
No one?

david_h April 11, 2007 10:10

To avoid an out of range error
 
To avoid an out of range error you might need to reduce your courant number below 0.5. Weller et. al. (Proc. of Comb. Inst. 1998) mention that a CFL < 0.5 is required for stability, CFL < 0.2 for accuracy. This has also been mentioned on the message board.

Are you using a fixed time-step or having the solver select a time-step based on a CFL condition ?

To alter the ignition you might try adding additional ignition sites and/or changing the parameters of the existing ignition sites.

Dave

arkangel April 26, 2007 04:18

Hi Thanks one last que
 
Hi

Thanks

one last question how can i do this
"having the solver select a time-step based on a CFL condition "

till a fixed time step

david_h April 26, 2007 09:54

To satisfy CFL < 0.2 you can m
 
To satisfy CFL < 0.2 you can make the following changes to "system/controlDict":

adjustTimeStep yes;
maxCo 0.2;

arkangel April 27, 2007 11:59

hi Thanks it is not working
 
hi Thanks

it is not working it is like i havent done anything , maybe i mistype something
here is my controlDict

application Xoodles;

startFrom startTime;

startTime 0;

stopAt endTime;

endTime 0.3;

deltaT 1e-05;

writeControl runTime;

writeInterval 0.005;

purgeWrite 0;

writeFormat ascii;

writePrecision 6;

writeCompression uncompressed;

timeFormat general;

timePrecision 6;

graphFormat raw;

runTimeModifiable yes;

adjustTimeStep yes;

maxCo 0.2;

lucchini April 27, 2007 12:04

Hi, what happens by using
 
Hi,

what happens by using maxCo 0.1? Is it crashing at the same point?

Try also to tighten the tolerances of the fvSolution by an order or two of magnitude and see what happens.

Bye

arkangel April 27, 2007 12:22

Hi Tommaso , David I mean I
 
Hi Tommaso , David

I mean I am not having control over the Time step, it is the same fiexed tiem step

but i am trying all your reomendations during this weekend

lucchini April 27, 2007 12:33

Hi again, the timeStep rem
 
Hi again,

the timeStep remains fixed because the Xoodles solver does not include the following lines in the time loop.


# include "readTimeControls.H"
# include "readPISOControls.H"

and after

# include "compressibleCourantNo.H"

also this one is needed

# include "setDeltaT.H"

Furthermore,

# include "setInitialDeltaT.H"

Should be pasted before the start of the time loop.

Try to have a look to the XiFoam application and then to the Xoodles application and try to put the correct files where needed to set the deltaT.

I hope I have been useful.

Bye

Tommaso

arkangel April 30, 2007 08:07

Hi Tommaso, thanks for your
 
Hi Tommaso,
thanks for your help i am testing now seems to be working

for someone else who might be interested
# include "readTimeControls.H"
should be placed before
# include "setInitialDeltaT.H" too

arkangel May 10, 2007 13:41

Hi me again ! I want to kno
 
Hi me again !

I want to know what is the relationship between these parameters in ignitions sites field:

duration 0.01;
strength 4;


I pretty sure that duration is the time in sec. during which the sparkle takes place. but if I am wrong (please correct me) . If I increase the duration time i also have to increase the strength in order to get the same result , the point is that i have no idea what is the relationship , what is the meaning of strength anyways

can someone enlighten me ?

lucchini May 10, 2007 17:04

Hi O R (?!?!) the ignition
 
Hi O R (?!?!)

the ignition treatment works as follows:

for its duration, a source term which is proportional to the strength is added to the equation for b. Have a look at the ignite.H file to know more about that.

Bye

Tommaso

arkangel May 14, 2007 08:28

Hi I am still having the s
 
Hi

I am still having the same error

FOAM FATAL ERROR : attempt to use janafThermo<equationofstate> out of temperature range 200 -> 5000; T = -736.126

the maxCo is 0.1 (in fact the last max Courant was 0.099034) the last residual for p, Ux, Uy,and k were 2.55e-08,2.44e-08,6.55e-09, 7.5e-10.

Something I can not still understand. In the previous time step the min temp either in T or Tu field were bigger than 200 , and in the next time step,(with a deltaT = 8.14815e-08 ) in one point the temperature simply dropped to -736.126 (how could this change happened in such small deltaT and Courant number)

and 3 time steps before the error i get Solution singularity for Xi and b , not sure if this is directly related , because I got the same singularity solution warning for Xi in the first Time Step

arkangel June 7, 2007 10:16

BUMP
 
BUMP

arkangel August 13, 2007 07:07

BUMP !! no one
 
BUMP !! no one

markusrehm August 14, 2007 03:28

Hello, I had the same error
 
Hello,

I had the same error using reactingFoam. I limited the enthalpy as suggested by Markus Hartinger (http://www.cfd-online.com/OpenFOAM_D...tml?1177099819). When I was at a certain stage I could continue my calculation with the (unlimited) standard solver.

Don't know if that might help.

Regards Markus

fox February 11, 2011 05:32

Hi Foamers,
im a new foamer and wondering if anybody has found a satisfying answer to the problem with the error from janafThermo:

Im currently working on a combustion induced vortex breakdown with XiFoam respectively myXiFoam (within this solver i have changed the calculation of the desity to be only depending on the compressibility) . Im using a 2D mesh (Axi-symmetric geometry using the wedge patch type) and running with low Courrant numbers 0.2<Co<0.5.

Anyway i get for both solvers the error message

-> FOAM FATAL ERROR: attempt to use janafThermo<equationOfState> out of temperature range 100 -> 5000; T = 99.3763

i have tryed to change Co number, fvSchemes (Crank-Nicholson, Upwind), time step and mesh density. So far, all attempts failed and I dont find any satisfying answer within the posts been made.

So please I would warmly and deeply appreciate any kind of help to solve this problem

greets


All times are GMT -4. The time now is 18:50.