I am trying to do the engineFo
I am trying to do the engineFoam tutorial (delivered with OpenFoam 1.2) but the application crashes all the time with the following error:
FOAM FATAL ERROR : attempt to use janafThermo<equationofstate> out of temperature range 200 -> 5000; T = 193.577
Ok with the default setup it crashes so I played a little bit with the parameters in fvSolution (increase non-orth and ncorrectors), controlDict (maxDeltaT=0.01, adjustTimeStep=yes) but with success (same error at other CA positions).
I think it would be very nice if the official tutorial will work "out of the box". For beginners it is quite impossible to know what parameters they have to change to run the case without these problems. Is there someone who has a setup for the engineFoam tutorial which works or is the tutorial just buggy?
Is there really nobody who can
Is there really nobody who can (would) help?
Hello, Did you use max. cou
Did you use max. courantno? and restarted the simulation from the beginning? (at least beginning of ignition?) It should work.
Yes I use the following: ad
Yes I use the following:
but it don`t work!
try to increase the number of
try to increase the number of piso loops and non-orthoganl corrections, try a 2/2, or 3/2 combo
thanks for helping me Niklas h
thanks for helping me Niklas http://www.cfd-online.com/OpenFOAM_D...part/happy.gif
I have already tried to increase the no of piso loops and non-orth corrections (tested with 2/2 3/2 3/6) but the problem still exists!
I have experienced the same pr
I have experienced the same problem as descirbed above!
Anyone out there who can help?
I'm experiencing also the same
I'm experiencing also the same problems. Changing the number of piso loops and non-ortogonal correctors delay the error, but it still exists. A differerent maxCo also has some effect, but the problem does not disappear.
When I look at the output in paraView it seems as if the error occurs when the combustion reaches the liner. Can anybody else confirm this?
Yes I agree, as soon as the fl
Yes I agree, as soon as the flame reaches the liner (approx 54CA) the solver blows up!
I have run this yesterday and
I have run this yesterday and it all works, all the way to 60 deg and full combustion. However, the spark plug location looks stupid to me, but that's another matter...
I will tar up the complete result for you and put it on http://powerlab.fsb.hr/ped/kturbo/OpenFOAM/ when I find a peaceful moment.
Thank you, The results are
The results are probably not that interesting, more interesting is the setup. Did you perform the simulation with fixedTemperatureWallFunctions or adiabaticWalls?, when I do the simulation with adiabaticWalls it also runs perfectly.
Here comes: You've got the
You've got the case with the complete solution zipped up in:
There's several IMPORTANT points I want to make:
- this is not the best mesh and the easiest physics to deal with.
- if I set up the second part to run with delta t of 0.01 degrees crank angle, everything runs smoothly and in one go. However, I am impatient and cannot be bothered to wait. Therefore...
- I have run a number of tests to see how the case fails, each time finding out why. In every single situation (when it fails), it fails because PISO stops converging, which is easy to spot and easy to fix.
Thus, when you are running your case, pay attention to the print out from the solver. PISO is that lot with several repetitions of:
solving for b
solving for Xi
solving for hu
solving for h
solving for p (several times)
Pay attention to the first initial residual in the "solving for p" bit: this tells you what PISO is doing. If in the last try you did not reduce the residual (INITIAL RESIDUAL) for at least an order of magnitude, your run is likely to blow up.
You can fix this in two ways:
- reduce the time-step. (you can always increase it later, when the combustion bit is finished
- increase the number of PISO correctors
- if your mesh is badly non-orthogonal, add non-orthogonal correctors or fiddle with the discretisation of the laplacian.
Now, I can set up this case and solver to be idiot-proof, with tons of PISO correctors, under-relaxation, time-step control and in a dozen more ways, but I cannot be bothered - I prefer to have people use their brain. Thus, please pay attention to what the solver is doing and act accordingly.
I appreciate that some people don't know this stuff or understand numerics. I would strongly recommend studying the code, reading about discretisation and thinking about stuff because otherwise you are likely to waste a lot of time staring into a black box.
If you are (really) interested, maybe we should consider doing a summer school or an intensive course on numerics (Finite Volume and CFD for starters), with OpenFOAM as a platform: this will not only teach you about algorithms but give you a chance to mess about with OpenFOAM solvers until you know them really well. If you're interested, please talk to me (I have done this before).
Enjoy the engine :-)
Hello! Could somebody direc
Could somebody direct me to a copy of the enginefoam tutorial ...
Hi hrv I am trying to run e
I am trying to run engine simulation on Openfoam. But The simpleEngineTutorial case is not running on my foam setup. what could be the possible reason for this? please guide me in this regard. Your suggestion posted above are helpful though. http://www.cfd-online.com/OpenFOAM_D...part/happy.gif
I am running in dieselFoam and also tried it on engineFoam. The error reported is:
[343880@w191-210 dieselFoam]$ paraFoam . simpleEngine
--> FOAM FATAL IO ERROR : keyword U is undefined in dictionary "/home/343880/OpenFOAM/343880-1.4.1/run/tutorials/dieselFoam/simpleEngine/215/p: :presin"
file: /home/343880/OpenFOAM/343880-1.4.1/run/tutorials/dieselFoam/simpleEngine/215/p:: presin from line 464 to line 466.
From function dictionary::lookupEntry(const word& keyword) const
in file db/dictionary/dictionary.C at line 146.
looking forward from you reply ..
Hi Nishant, this is due to
this is due to a change in the totalPressure boundary condition dictionary. Modify it as follows:
p0 uniform 0;
value uniform 0;
And it will work.
Please specify the correct value for the entries "value" and "p0" (here I put 0 just as an example)
Hope this can help.
Hi Tommaso Thanks for the re
Thanks for the response.
Actually my boundary files in dir "-225" is - see attachment.
i am not sure which value i am supposed to change. can u please point it out.
I have the same problem with OpenFOAM-1.5. I tried to make an example, that is described in programmers guide. But I have an error
keyword PISO is undefined in dictionary "/home/caelinux/OpenFOAM/caelinux-1.5/run/tutorials/simpleFoam/pitzDaily/system/fvSolution"
file: /home/caelinux/OpenFOAM/caelinux-1.5/run/tutorials/simpleFoam/pitzDaily/system/fvSolution from line 19 to line 69.
From function dictionary::subDict(const word& keyword) const
I'm waiting for your reply=)
Sorry to dig up the thread, but I kinda have the same problem and i can't figure out what's wrong..
I have both OF1.7.1 and 2.1.1, and i'm trying to use engineFoam. I've checked every file in both tutorial cases, and they are exactly the same (except for some keywords syntax, but no big deal making the link between the two versions).
For the 2.1.1 case/solver, I've lowered maxCo, increased the number of correctors,.. followed every advice in this thread, but pressure and Temperature are still decreasing and temperature eventually gets out of janaf tables range...
But with the 1.7.1 solver, everything's working just fine (except for pressure and temperature a bit to low near TDC, as opposed to classical SI engine values, but someone already mentioned it in another thread and that's not the point...)
Does anyone experience the same problem?
Is there something 'wrong' with the new engineFoam solver or with the tutorial case? (btw, sprayEngineFoam has the same problem...)
Greetings Gregory and welcome to the forum!
Which exact tutorial are you using?
There have been changes in the diesel and engine solvers for a while now, due to some issues... I'll have to dig up some dirt to find the issues on this topic... here we go:
|All times are GMT -4. The time now is 07:32.|