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

Error using kOmegaSST in sprayFoam

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

Like Tree1Likes
  • 1 Post By CFDUser_

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   April 17, 2014, 06:01
Default Error using kOmegaSST in sprayFoam
  #1
Member
 
CFDUser
Join Date: Mar 2014
Posts: 59
Rep Power: 13
CFDUser_ is on a distinguished road
Hi All,
Hope everyone is good.
I got the following error while running sprayFoam for kOmegaSST turbulent model.
Code:
--> FOAM FATAL ERROR: 

    lookup of turbulenceModel from objectRegistry region0 successful
    but it is not a turbulenceModel, it is a kOmegaSST

    From function objectRegistry::lookupObject<Type>(const word&) const
    in file /home/opencfd/OpenFOAM/OpenFOAM-2.3.0/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 181.

FOAM aborting

#0  Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam230/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1  Foam::error::abort() in "/opt/openfoam230/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2  Foam::incompressible::turbulenceModel const& Foam::objectRegistry::lookupObject<Foam::incompressible::turbulenceModel>(Foam::word const&) const in "/opt/openfoam230/platforms/linux64GccDPOpt/lib/liblagrangianTurbulence.so"
#3  Foam::incompressible::omegaWallFunctionFvPatchScalarField::updateCoeffs() in "/opt/openfoam230/platforms/linux64GccDPOpt/lib/libincompressibleRASModels.so"
#4  Foam::compressible::RASModels::kOmegaSST::correct() in "/opt/openfoam230/platforms/linux64GccDPOpt/lib/libcompressibleRASModels.so"
#5  

#6  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#7  

Aborted (core dumped)
Its weird but ya its true. it is saying kOmegaSST is not turbulent model.
Still unable to figure out how to correct it. It is failing to register RASModel (run time constructor for RASModel). I know that PISO is most generic for turbulence models in OpenFOAM and sprayFoam is derived from PISO. So, problem should be some where else (I mean not in constructing RASModel). I am unable to figure it out. Can some body help me?

All I have done to get this error Is replaced aachenBomb geometry with simple square duct then specified proper BCs to run flow problem. Worked well with kEpsilon. Then changed turbulence model to kOmegaSST.

Regards,
CFDUser_
CFDUser_ is offline   Reply With Quote

Old   April 18, 2014, 03:51
Default
  #2
Senior Member
 
Tom Fahner
Join Date: Mar 2009
Location: Breda, Netherlands
Posts: 646
Rep Power: 32
tomf will become famous soon enoughtomf will become famous soon enough
Send a message via MSN to tomf Send a message via Skype™ to tomf
Could you provide the turbulenceProperties and RASProperties files you used? I am guessing from your information something is incorrectly set there. Regards, Tom
tomf is offline   Reply With Quote

Old   April 18, 2014, 04:29
Default
  #3
Member
 
CFDUser
Join Date: Mar 2014
Posts: 59
Rep Power: 13
CFDUser_ is on a distinguished road
Quote:
Originally Posted by tomf View Post
Could you provide the turbulenceProperties and RASProperties files you used? I am guessing from your information something is incorrectly set there. Regards, Tom
Hi Tom,

Thanks for the reply.
Details you asked are furnished below
RASProperties:
RASModel kOmegaSST;
turbulence on;
printCoeffs on;

turbulenceproperties:
simulationType RASModel;


Regards,
CFDUser_
CFDUser_ is offline   Reply With Quote

Old   April 18, 2014, 04:51
Default
  #4
Senior Member
 
Tom Fahner
Join Date: Mar 2009
Location: Breda, Netherlands
Posts: 646
Rep Power: 32
tomf will become famous soon enoughtomf will become famous soon enough
Send a message via MSN to tomf Send a message via Skype™ to tomf
Maybe there is something in the header above this information that is incorrectly set? So could you just output the entire file contents?

Otherwise it may be a bug in version 2.3.0?

I just changed the turbulence model to kOmegaSST in the copied aachenBomb tutorial for 2.3.x.

It runs fine and is attached:

simply do:

Code:
$> blockMesh
$> sprayFoam
Just copied epsilon to omega and kept the values, so maybe it is incorrect, but it runs at least.
Attached Files
File Type: gz aachenBomb.tar.gz (5.4 KB, 28 views)
tomf is offline   Reply With Quote

Old   April 18, 2014, 04:57
Default
  #5
Member
 
CFDUser
Join Date: Mar 2014
Posts: 59
Rep Power: 13
CFDUser_ is on a distinguished road
Quote:
Originally Posted by tomf View Post
Maybe there is something in the header above this information that is incorrectly set? So could you just output the entire file contents?

Otherwise it may be a bug in version 2.3.0?

I just changed the turbulence model to kOmegaSST in the copied aachenBomb tutorial for 2.3.x.

It runs fine and is attached:

simply do:

Code:
$> blockMesh
$> sprayFoam
Just copied epsilon to omega and kept the values, so maybe it is incorrect, but it runs at least.
I did this already and succeed. problem arrived when tried to change the case to flow problem.
Why don't you change your case to simple flow problem(floe through simple square duct may be) and try the same.

Regards,
CFDUser_
CFDUser_ is offline   Reply With Quote

Old   April 18, 2014, 05:09
Default
  #6
Senior Member
 
Tom Fahner
Join Date: Mar 2009
Location: Breda, Netherlands
Posts: 646
Rep Power: 32
tomf will become famous soon enoughtomf will become famous soon enough
Send a message via MSN to tomf Send a message via Skype™ to tomf
I will not have that amount of time available at the moment I am afraid, maybe some one else has. Probably best if you can provide the case that is troubling you so someone can have a look at it. We do not know what you have in front of you exactly.
tomf is offline   Reply With Quote

Old   April 19, 2014, 04:18
Default
  #7
Member
 
CFDUser
Join Date: Mar 2014
Posts: 59
Rep Power: 13
CFDUser_ is on a distinguished road
Quote:
Originally Posted by tomf View Post
I will not have that amount of time available at the moment I am afraid, maybe some one else has. Probably best if you can provide the case that is troubling you so someone can have a look at it. We do not know what you have in front of you exactly.
Dear Tom,

Thanks for your support. There was no bug. I gave wrong input for omega.
Now its working.

Thanks a lot.

Regards,
CFDUser_
CFDUser_ is offline   Reply With Quote

Old   July 1, 2014, 10:55
Default
  #8
New Member
 
Join Date: Jul 2014
Posts: 6
Rep Power: 12
appie is on a distinguished road
Quote:
Originally Posted by CFDUser_ View Post
Dear Tom,

Thanks for your support. There was no bug. I gave wrong input for omega.
Now its working.

Thanks a lot.

Regards,
CFDUser_
Dear CFDUser,

I'd be interested to know how you saw that the input for omega was incorrect?

And what did you change to solve it?

I'm encountering the same error...

Many thanks in advance!
appie is offline   Reply With Quote

Old   July 1, 2014, 11:08
Default
  #9
Member
 
CFDUser
Join Date: Mar 2014
Posts: 59
Rep Power: 13
CFDUser_ is on a distinguished road
Quote:
Originally Posted by appie View Post
Dear CFDUser,

I'd be interested to know how you saw that the input for omega was incorrect?

And what did you change to solve it?

I'm encountering the same error...

Many thanks in advance!
Are you solving for compressible flow and your omega type is just omegaWallFunction??

just change type to compressible:megaWallFunction in omega file.

Your are done.

Regards,
CFDUser_
Eldrael likes this.
CFDUser_ is offline   Reply With Quote

Old   July 1, 2014, 11:23
Default
  #10
New Member
 
Join Date: Jul 2014
Posts: 6
Rep Power: 12
appie is on a distinguished road
Wow, thanks for the quick reply.

It's a bit different. I'm changing my case from a compressible solver to an incompressible. I'm not sure where the error originates, but I make it till here:

DILUPBiCG: Solving for Ux, Initial residual = 0.999999999998, Final residual = 2.60220350182e-08, No Iterations 4
DILUPBiCG: Solving for Uy, Initial residual = 0.999999999987, Final residual = 3.46113359058e-08, No Iterations 4
DILUPBiCG: Solving for Uz, Initial residual = 0.999999999999, Final residual = 3.1130707825e-08, No Iterations 4
DILUPBiCG: Solving for H2O, Initial residual = 0.999999891847, Final residual = 5.29106562959e-09, No Iterations 3
DILUPBiCG: Solving for CO2, Initial residual = 5.87534515923e-05, Final residual = 5.55965647659e-08, No Iterations 1


--> FOAM FATAL ERROR:

lookup of turbulenceModel from objectRegistry region0 successful
but it is not a turbulenceModel, it is a realizableKE


The enthalpy(h) is the next equation to be solved, so I would think T so be the source of error. I switched the B.C. between compressible::turbulentHeatFluxTemperature and turbulentHeatFluxTemperature.

I'll continue battling this error, and get be to be more clear...

Regards,

Appie
appie is offline   Reply With Quote

Old   July 1, 2014, 13:01
Default
  #11
Member
 
CFDUser
Join Date: Mar 2014
Posts: 59
Rep Power: 13
CFDUser_ is on a distinguished road
Quote:
Originally Posted by appie View Post
Wow, thanks for the quick reply.

It's a bit different. I'm changing my case from a compressible solver to an incompressible. I'm not sure where the error originates, but I make it till here:

DILUPBiCG: Solving for Ux, Initial residual = 0.999999999998, Final residual = 2.60220350182e-08, No Iterations 4
DILUPBiCG: Solving for Uy, Initial residual = 0.999999999987, Final residual = 3.46113359058e-08, No Iterations 4
DILUPBiCG: Solving for Uz, Initial residual = 0.999999999999, Final residual = 3.1130707825e-08, No Iterations 4
DILUPBiCG: Solving for H2O, Initial residual = 0.999999891847, Final residual = 5.29106562959e-09, No Iterations 3
DILUPBiCG: Solving for CO2, Initial residual = 5.87534515923e-05, Final residual = 5.55965647659e-08, No Iterations 1


--> FOAM FATAL ERROR:

lookup of turbulenceModel from objectRegistry region0 successful
but it is not a turbulenceModel, it is a realizableKE


The enthalpy(h) is the next equation to be solved, so I would think T so be the source of error. I switched the B.C. between compressible::turbulentHeatFluxTemperature and turbulentHeatFluxTemperature.

I'll continue battling this error, and get be to be more clear...

Regards,

Appie
Check all your bc's. May be you are specifying some other field as compressible.


CFDUser_
CFDUser_ is offline   Reply With Quote

Old   July 2, 2014, 03:38
Default
  #12
New Member
 
Join Date: Jul 2014
Posts: 6
Rep Power: 12
appie is on a distinguished road
Thanks, you were right. Thanks for the help!

I had wallHeatTransfer instead of incompessibleWallHeatTransfer..
appie is offline   Reply With Quote

Old   March 12, 2015, 20:43
Default Help accepted
  #13
Member
 
Jairo A. Gutiérrez S
Join Date: Nov 2014
Posts: 60
Rep Power: 11
jairoandres is on a distinguished road
Dear Foamers... I am having a similar issue than CFDUSER___ I replaced the AachenBomb tutorial with a modified spray (that I already tested), and finally I added flow with the proper boundary conditions... However i am having an error I havent figured.... It comes after calculating the first step for most variables (after rho), I have read of bugs with sprayfoam and kepsilon but i've read that this worked for CFDUSER .... Can i have any guess of the issue on this??
diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 7.99435e-09, global = -1.24757e-09, cumulative = -3.71235e-05
#0 Foam::error:rintStack(Foam::Ostream&) at ??:?
#1 Foam::sigFpe::sigHandler(int) at ??:?
#2 in "/lib/x86_64-linux-gnu/libc.so.6"
#3 Foam::divide(Foam::Field<double>&, Foam::UList<double> const&, Foam::UList<double> const&) at ??:?
#4 void Foam::divide<Foam::fvsPatchField, Foam::surfaceMesh>(Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh>&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&) at ??:?
#5 Foam::tmp<Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> > Foam:perator/<Foam::fvsPatchField, Foam::surfaceMesh>(Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::tmp<Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> > const&) at ??:?
#6 Foam::compressible::RASModels::kEpsilon::correct() at ??:?
#7
at ??:?
#8 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#9
at ??:?
Floating point exception (core dumped)
jairoandres is offline   Reply With Quote

Old   March 13, 2015, 01:14
Default
  #14
Member
 
Lucas Mutti
Join Date: Aug 2013
Posts: 47
Rep Power: 14
lramutti is on a distinguished road
Division by zero. Somewhere in your 0 or systems folder - depending what solver you are using (i.e. conjugate heat transfer) - has a zero value boundary/ initial condition. Might be worth it to take a look.

Cheers

-Lucas
lramutti is offline   Reply With Quote

Old   March 13, 2015, 10:32
Default Hi
  #15
Member
 
Jairo A. Gutiérrez S
Join Date: Nov 2014
Posts: 60
Rep Power: 11
jairoandres is on a distinguished road
Thanks for your answer... I figured the same, however I wouldnt expect any issues since I replaced Aachenbomb and added inlet and oulet boundaries...After giving it a big though I think I know where is this heading into... sprayFoam.c says it handles energy instead of temperature as a transport equation. Since there were no inlets / outlets of energy in Aachenbomb as boundary conditions I guess they didnt use an EEqn.h (because it was not necessary). However if I add flow, the flow has enthalpy on it and it becomes a source in time=0, and maybe this is creating the error. I will check everything then add this and will tell you... Thanks again
jairoandres is offline   Reply With Quote

Old   March 13, 2015, 14:30
Default
  #16
Member
 
Lucas Mutti
Join Date: Aug 2013
Posts: 47
Rep Power: 14
lramutti is on a distinguished road
Now that you mentioned I recall that I had a similar problem. In order for you to run the SST k omega model you must define some parameters. If I remember correctly the equation considers the division of a factor which I believe it is labeled as B while calculating the F or F-max values. Might be worth it to confirm what values those parameters take and check if this solves the problem. If its set as 0 just make them infinitesimally small.

Hope that helps

Lucas
lramutti is offline   Reply With Quote

Old   May 5, 2015, 16:30
Default sprayfoam with convective flow
  #17
Member
 
Jairo A. Gutiérrez S
Join Date: Nov 2014
Posts: 60
Rep Power: 11
jairoandres is on a distinguished road
Ok it worked for me at last.... Thank you all... some advice for the new guys...

1) Sprayfoam looks to be only a compressible flow solver. one of the errors i had was because i changed the wall functions to incompressible.

2) I was used to set pressure outlet to 0 in the boundary for 0-p. But of course since solver is compressible this will get a big error..

3) Something logical, but sometimes u dont see it because i was migrating from simplefoam... use mut instead of nut. Otherwise you will have dimensional problems.
jairoandres is offline   Reply With Quote

Old   November 20, 2023, 16:29
Default
  #18
New Member
 
Join Date: Nov 2023
Posts: 2
Rep Power: 0
StefanosTrat is on a distinguished road
hello foamers, kinda similar problem here , cant understand it because in cumbustion properties i have set the model PaSR

--> FOAM FATAL ERROR:
[3]
lookup of combustionProperties from objectRegistry region0 successful
but it is not a CombustionModel<rhoReactionThermo>, it is a PaSR<psiReactionThermo>
[3]
[3] From function const Type& Foam:bjectRegistry::lookupObject(const Foam::word&) const [with Type = Foam::combustionModels::singleStepCombustion<Foam: :rhoReactionThermo, Foam::sutherlandTransport<Foam::species::thermo<Fo am::janafThermo<Foam:erfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > >]
StefanosTrat is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
manualInjection model in sprayFoam Mentalo OpenFOAM Running, Solving & CFD 1 April 2, 2014 10:29
sprayFoam crashes lukasfischer OpenFOAM Running, Solving & CFD 3 July 14, 2013 12:08
kOmegaSST OF2.1 Help needed! wiedangel OpenFOAM Running, Solving & CFD 0 May 9, 2012 11:01
Wrong calculation of nut in the kOmegaSST turbulence model FelixL OpenFOAM Bugs 27 March 27, 2012 10:02
kOmegaSST in openfoam 1.6 Gearb0x OpenFOAM 2 March 3, 2010 07:02


All times are GMT -4. The time now is 15:26.