CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

Weird problem with engineFoam tutorial

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree1Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   February 3, 2006, 08:01
Default I am trying to do the engineFo
  #1
Member
 
chris book
Join Date: Mar 2009
Posts: 85
Rep Power: 8
chris1980 is on a distinguished road
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?
chris1980 is offline   Reply With Quote

Old   February 7, 2006, 10:53
Default Is there really nobody who can
  #2
Member
 
chris book
Join Date: Mar 2009
Posts: 85
Rep Power: 8
chris1980 is on a distinguished road
Is there really nobody who can (would) help?
chris1980 is offline   Reply With Quote

Old   February 7, 2006, 11:37
Default Hello, Did you use max. cou
  #3
Member
 
Guido Adriaensen
Join Date: Mar 2009
Posts: 56
Rep Power: 8
guido_adriaensen is on a distinguished road
Hello,

Did you use max. courantno? and restarted the simulation from the beginning? (at least beginning of ignition?) It should work.

regards
Guido
guido_adriaensen is offline   Reply With Quote

Old   February 7, 2006, 11:42
Default Yes I use the following: ad
  #4
Member
 
chris book
Join Date: Mar 2009
Posts: 85
Rep Power: 8
chris1980 is on a distinguished road
Yes I use the following:

adjustTimeStep yes
maxCo 0.2
maxDeltaT 0.025

but it don`t work!
chris1980 is offline   Reply With Quote

Old   February 7, 2006, 16:23
Default try to increase the number of
  #5
Super Moderator
 
niklas's Avatar
 
Niklas Nordin
Join Date: Mar 2009
Location: Stockholm, Sweden
Posts: 693
Rep Power: 19
niklas will become famous soon enough
try to increase the number of piso loops and non-orthoganl corrections, try a 2/2, or 3/2 combo
niklas is offline   Reply With Quote

Old   February 8, 2006, 03:23
Default thanks for helping me Niklas h
  #6
Member
 
chris book
Join Date: Mar 2009
Posts: 85
Rep Power: 8
chris1980 is on a distinguished road
thanks for helping me Niklas

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!
chris1980 is offline   Reply With Quote

Old   February 9, 2006, 05:55
Default I have experienced the same pr
  #7
Member
 
stefan
Join Date: Mar 2009
Posts: 96
Rep Power: 8
stefanke is on a distinguished road
I have experienced the same problem as descirbed above!

Anyone out there who can help?
stefanke is offline   Reply With Quote

Old   February 9, 2006, 11:12
Default I'm experiencing also the same
  #8
Member
 
Guido Adriaensen
Join Date: Mar 2009
Posts: 56
Rep Power: 8
guido_adriaensen is on a distinguished road
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?

Guido
guido_adriaensen is offline   Reply With Quote

Old   February 9, 2006, 11:19
Default Yes I agree, as soon as the fl
  #9
Member
 
stefan
Join Date: Mar 2009
Posts: 96
Rep Power: 8
stefanke is on a distinguished road
Yes I agree, as soon as the flame reaches the liner (approx 54CA) the solver blows up!
stefanke is offline   Reply With Quote

Old   February 9, 2006, 11:24
Default I have run this yesterday and
  #10
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
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.

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   February 9, 2006, 11:36
Default Thank you, The results are
  #11
Member
 
Guido Adriaensen
Join Date: Mar 2009
Posts: 56
Rep Power: 8
guido_adriaensen is on a distinguished road
Thank you,

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.

Guido
guido_adriaensen is offline   Reply With Quote

Old   February 9, 2006, 20:02
Default Here comes: You've got the
  #12
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
Here comes:

You've got the case with the complete solution zipped up in:

http://powerlab.fsb.hr/ped/kturbo/OpenFOAM/

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 :-)

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   January 13, 2007, 14:37
Default Hello! Could somebody direc
  #13
New Member
 
N S Prasad
Join Date: Mar 2009
Posts: 15
Rep Power: 8
nsp82 is on a distinguished road
Hello!

Could somebody direct me to a copy of the enginefoam tutorial ...

Thanks.
nsp82 is offline   Reply With Quote

Old   December 19, 2007, 17:42
Default Hi hrv I am trying to run e
  #14
Senior Member
 
Nishant
Join Date: Mar 2009
Location: Glasgow, UK
Posts: 165
Rep Power: 8
nishant_hull is on a distinguished road
Hi hrv

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.
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.

FOAM exiting



looking forward from you reply ..

Nishant
__________________
Thanks and regards,

Nishant
nishant_hull is offline   Reply With Quote

Old   December 19, 2007, 18:05
Default Hi Nishant, this is due to
  #15
Member
 
Tommaso Lucchini
Join Date: Mar 2009
Posts: 82
Rep Power: 8
lucchini is on a distinguished road
Hi Nishant,

this is due to a change in the totalPressure boundary condition dictionary. Modify it as follows:



type totalPressure;
p0 uniform 0;
U U;
phi phi;
rho none;
psi none;
gamma 1.0;
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.

Regards

Tommaso
lucchini is offline   Reply With Quote

Old   December 19, 2007, 18:59
Default Hi Tommaso Thanks for the re
  #16
Senior Member
 
Nishant
Join Date: Mar 2009
Location: Glasgow, UK
Posts: 165
Rep Power: 8
nishant_hull is on a distinguished road
Hi Tommaso
Thanks for the response.
Actually my boundary files in dir "-225" is - see attachment.
\attach
i am not sure which value i am supposed to change. can u please point it out.

Nishant
__________________
Thanks and regards,

Nishant
nishant_hull is offline   Reply With Quote

Old   December 19, 2007, 19:00
Default http://www.cfd-online.com/Ope
  #17
Senior Member
 
Nishant
Join Date: Mar 2009
Location: Glasgow, UK
Posts: 165
Rep Power: 8
nishant_hull is on a distinguished road
p
__________________
Thanks and regards,

Nishant
nishant_hull is offline   Reply With Quote

Old   October 2, 2009, 07:02
Default
  #18
Member
 
Arina
Join Date: Oct 2009
Location: Belarus
Posts: 76
Rep Power: 7
Akuji is on a distinguished road
Send a message via ICQ to Akuji
Hello,
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=)
Akuji is offline   Reply With Quote

Old   July 17, 2012, 09:55
Default
  #19
New Member
 
Gregory Paladin
Join Date: Jul 2012
Posts: 10
Rep Power: 4
paladin is on a distinguished road
Quote:
Originally Posted by chris1980 View Post
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?


Hi,

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...)


Thanks !

Gregory
paladin is offline   Reply With Quote

Old   July 17, 2012, 15:42
Default
  #20
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,251
Blog Entries: 34
Rep Power: 84
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
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:
Best regards,
Bruno
wyldckat is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Parallel run with engineFoam francesco OpenFOAM Running, Solving & CFD 4 October 5, 2014 15:49
Refining mesh in engineFoam johan OpenFOAM Mesh Utilities 1 December 2, 2008 04:58
Parallel run with engineFoam francesco OpenFOAM Bugs 1 November 25, 2008 08:06
Really weird problem could nbt figure it out 21kalee OpenFOAM Running, Solving & CFD 2 December 30, 2007 11:30
Line/Rake - Weird Problem Marc FLUENT 6 August 8, 2007 14:15


All times are GMT -4. The time now is 17:32.