passive scalar increases

immortality · May 23, 2013, 06:57

Hi again before close the issue dossier!
when I used linear scheme for probably more accuracy it didn't get a good result(not good appearance and also higher than 1)

Code:

div(phi,gas) Gauss linear;

but in upwind worked well again.
the question is:why its so?!

Tobi · May 23, 2013, 07:15

Quote:

Originally Posted by immortality

Hi again before close the issue dossier!
when I used linear scheme for probably more accuracy it didn't get a good result(not good appearance and also higher than 1)
[CODEdiv(phi,gas) Gauss linear;][/CODE]
but in upwind worked well again.
the question is:why its so?!

That depend on the schemes. On my Homepage you can find a summary about that Topic (unfortunatelly only in german). But the grapics show everything I think.

http://www.holzmann-cfd.de/index.php...rische-schemen

Tobi · May 23, 2013, 07:21

Info about the added Lines: Sp(...)

-> http://www.cfd-online.com/Forums/ope...tml#post407482

immortality · May 23, 2013, 08:18

thanks Tobias
related to vanLeer nothing has said but it has nice results,then what do you suggest for better accurate and physical results for passive scalar transport?

Tobi · May 23, 2013, 11:44

Quote:

Originally Posted by immortality

thanks Tobias
related to vanLeer nothing has said but it has nice results,then what do you suggest for better accurate and physical results for passive scalar transport?

I always prefer 2. order schemes.

For the scalar I prefer

Code:

limitedLimitedLinear 1 0 1

immortality · May 23, 2013, 14:45

thanks.
vanLeer isn't a second order scheme?
what do 1 0 1 refer to respectively in the scheme?

Tobi · May 23, 2013, 15:05

vanLeer is a second order scheme.

To prevent unphysical results (the only scheme which is not producing unphysical results is gauss upwind 1st order) you can use limited schemes and schemes that are bouding the values:

Code:

 
limtiedLinear 1
limitedLinear 0.33
limitedLinear 0 = linear

The number behind the name is the value of the lmiiter. If you set it to one you have full limited functionallity. If you set it to zero there is no limiting in the scheme so you have the normal linear scheme.

Code:

limitedLimitedLinear 1 0 1

- first number is for the limiter function as befor

- the second one is the lower bouding value
- the third one is the upper bouding value

As you set your scalar between 0-13.54 you should write:

Code:

limitedLimitedLinear 1 0 13.54

immortality · May 23, 2013, 15:21

thank you for your full clarification.

immortality · May 25, 2013, 16:16

Hi again!
and what will be the proper code for an incompressible case? I wrote sp(rho,gas) in pimpleFoam and it got an error and when removed rho from equation in got another error:http://www.cfd-online.com/Forums/ope...tml#post430020
so whats the correct equation?

Tobi · May 26, 2013, 04:17

Quote:

Originally Posted by immortality

Hi again!
and what will be the proper code for an incompressible case? I wrote sp(rho,gas) in pimpleFoam and it got an error and when removed rho from equation in got another error:http://www.cfd-online.com/Forums/ope...tml#post430020
so whats the correct equation?

Hi

Code:

ddt(phi, gas)

should work

immortality · May 26, 2013, 05:30

Hi,sure it needs to be modified:

Code:

fvScalarMatrix gasEqn
	(
	  fvm::ddt(phi,gas)
         -fvm::Sp(phi, gas)
         +fvm::div(phi, gas)
         -fvm::Sp(fvc::div(phi), gas)
         -fvm::laplacian(turbulence->nuEff(), gas)
	);
	
	gasEqn.relax();
	gasEqn.solve(mesh.solver("gas"));

this error occurred:

Code:

Making dependency list for source file pimpleFoamModified.C
SOURCE=pimpleFoamModified.C ;  g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3  -DNoRepository -ftemplate-depth-100 -I/opt/openfoam220/src/turbulenceModels/incompressible/turbulenceModel -I/opt/openfoam220/src/transportModels -I/opt/openfoam220/src/transportModels/incompressible/singlePhaseTransportModel -I/opt/openfoam220/src/finiteVolume/lnInclude -I/opt/openfoam220/src/meshTools/lnInclude -I/opt/openfoam220/src/fvOptions/lnInclude -I/opt/openfoam220/src/sampling/lnInclude -IlnInclude -I. -I/opt/openfoam220/src/OpenFOAM/lnInclude -I/opt/openfoam220/src/OSspecific/POSIX/lnInclude   -fPIC -c $SOURCE -o Make/linux64GccDPOpt/pimpleFoamModified.o
In file included from pimpleFoamModified.C:89:0:
gasEqn.H: In function ‘int main(int, char**)’:
gasEqn.H:5:20: error: no matching function for call to ‘ddt(Foam::surfaceScalarField&, Foam::volScalarField&)’
gasEqn.H:5:20: note: candidates are:
/opt/openfoam220/src/finiteVolume/lnInclude/fvmDdt.C:45:1: note: template<class Type> Foam::tmp<Foam::fvMatrix<Type> > Foam::fvm::ddt(const Foam::GeometricField<Type, Foam::fvPatchField, Foam::volMesh>&)
/opt/openfoam220/src/finiteVolume/lnInclude/fvmDdt.C:60:1: note: template<class Type> Foam::tmp<Foam::fvMatrix<Type> > Foam::fvm::ddt(const Foam::one&, const Foam::GeometricField<Type, Foam::fvPatchField, Foam::volMesh>&)
/opt/openfoam220/src/finiteVolume/lnInclude/fvmDdt.C:72:1: note: template<class Type> Foam::tmp<Foam::fvMatrix<Type> > Foam::fvm::ddt(const dimensionedScalar&, const Foam::GeometricField<Type, Foam::fvPatchField, Foam::volMesh>&)
/opt/openfoam220/src/finiteVolume/lnInclude/fvmDdt.C:88:1: note: template<class Type> Foam::tmp<Foam::fvMatrix<Type> > Foam::fvm::ddt(const volScalarField&, const Foam::GeometricField<Type, Foam::fvPatchField, Foam::volMesh>&)
gasEqn.H:6:27: error: no matching function for call to ‘Sp(Foam::surfaceScalarField&, Foam::volScalarField&)’
gasEqn.H:6:27: note: candidates are:
/opt/openfoam220/src/finiteVolume/lnInclude/fvmSup.C:100:1: note: template<class Type> Foam::tmp<Foam::fvMatrix<Type> > Foam::fvm::Sp(const Foam::DimensionedField<double, Foam::volMesh>&, const Foam::GeometricField<Type, Foam::fvPatchField, Foam::volMesh>&)
/opt/openfoam220/src/finiteVolume/lnInclude/fvmSup.C:126:1: note: template<class Type> Foam::tmp<Foam::fvMatrix<Type> > Foam::fvm::Sp(const Foam::tmp<Foam::DimensionedField<double, Foam::volMesh> >&, const Foam::GeometricField<Type, Foam::fvPatchField, Foam::volMesh>&)
/opt/openfoam220/src/finiteVolume/lnInclude/fvmSup.C:140:1: note: template<class Type> Foam::tmp<Foam::fvMatrix<Type> > Foam::fvm::Sp(const Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> >&, const Foam::GeometricField<Type, Foam::fvPatchField, Foam::volMesh>&)
/opt/openfoam220/src/finiteVolume/lnInclude/fvmSup.C:154:1: note: template<class Type> Foam::tmp<Foam::fvMatrix<Type> > Foam::fvm::Sp(const dimensionedScalar&, const Foam::GeometricField<Type, Foam::fvPatchField, Foam::volMesh>&)
/opt/openfoam220/src/finiteVolume/lnInclude/fvmSup.C:180:1: note: template<class Type> Foam::zeroField Foam::fvm::Sp(const Foam::zero&, const Foam::GeometricField<Type, Foam::fvPatchField, Foam::volMesh>&)
make: *** [Make/linux64GccDPOpt/pimpleFoamModified.o] Error 1

Tobi · May 26, 2013, 13:18

Sorry... my fault:

Code:

fvm::ddt(gas)

immortality · May 26, 2013, 13:52

Hi tobias
I changed it:

Code:

fvScalarMatrix gasEqn
	(
	  fvm::ddt(gas)
         -fvm::Sp(phi, gas)
         +fvm::div(phi, gas)
         -fvm::Sp(fvc::div(phi), gas)
         -fvm::laplacian(turbulence->nuEff(), gas)
	);
	
	gasEqn.relax();
	gasEqn.solve(mesh.solver("gas"));

but the error persists:

Code:

ehsan@Ehsan-com:~/Desktop/Solvers/pimpleFoamModified$ wmake
Making dependency list for source file pimpleFoamModified.C
SOURCE=pimpleFoamModified.C ;  g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3  -DNoRepository -ftemplate-depth-100 -I/opt/openfoam220/src/turbulenceModels/incompressible/turbulenceModel -I/opt/openfoam220/src/transportModels -I/opt/openfoam220/src/transportModels/incompressible/singlePhaseTransportModel -I/opt/openfoam220/src/finiteVolume/lnInclude -I/opt/openfoam220/src/meshTools/lnInclude -I/opt/openfoam220/src/fvOptions/lnInclude -I/opt/openfoam220/src/sampling/lnInclude -IlnInclude -I. -I/opt/openfoam220/src/OpenFOAM/lnInclude -I/opt/openfoam220/src/OSspecific/POSIX/lnInclude   -fPIC -c $SOURCE -o Make/linux64GccDPOpt/pimpleFoamModified.o
In file included from pimpleFoamModified.C:89:0:
gasEqn.H: In function ‘int main(int, char**)’:
gasEqn.H:6:27: error: no matching function for call to ‘Sp(Foam::surfaceScalarField&, Foam::volScalarField&)’
gasEqn.H:6:27: note: candidates are:
/opt/openfoam220/src/finiteVolume/lnInclude/fvmSup.C:100:1: note: template<class Type> Foam::tmp<Foam::fvMatrix<Type> > Foam::fvm::Sp(const Foam::DimensionedField<double, Foam::volMesh>&, const Foam::GeometricField<Type, Foam::fvPatchField, Foam::volMesh>&)
/opt/openfoam220/src/finiteVolume/lnInclude/fvmSup.C:126:1: note: template<class Type> Foam::tmp<Foam::fvMatrix<Type> > Foam::fvm::Sp(const Foam::tmp<Foam::DimensionedField<double, Foam::volMesh> >&, const Foam::GeometricField<Type, Foam::fvPatchField, Foam::volMesh>&)
/opt/openfoam220/src/finiteVolume/lnInclude/fvmSup.C:140:1: note: template<class Type> Foam::tmp<Foam::fvMatrix<Type> > Foam::fvm::Sp(const Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> >&, const Foam::GeometricField<Type, Foam::fvPatchField, Foam::volMesh>&)
/opt/openfoam220/src/finiteVolume/lnInclude/fvmSup.C:154:1: note: template<class Type> Foam::tmp<Foam::fvMatrix<Type> > Foam::fvm::Sp(const dimensionedScalar&, const Foam::GeometricField<Type, Foam::fvPatchField, Foam::volMesh>&)
/opt/openfoam220/src/finiteVolume/lnInclude/fvmSup.C:180:1: note: template<class Type> Foam::zeroField Foam::fvm::Sp(const Foam::zero&, const Foam::GeometricField<Type, Foam::fvPatchField, Foam::volMesh>&)
make: *** [Make/linux64GccDPOpt/pimpleFoamModified.o] Error 1

maybe the Sp term should be removed?
I don't know yet exactly when we have to use Sp term.could you please clarify again for me?

immortality · December 25, 2013, 10:46

Hi dear Tobias
this link has been broken,could you give me another link for referencing? thanks.
http://www.holzmann-cfd.de/index.php...rische-schemen

wyldckat · December 25, 2013, 12:03

Greetings to all!

@Ehsan:

Quote:

Originally Posted by immortality

Hi dear Tobias
this link has been broken,could you give me another link for referencing? thanks.
http://www.holzmann-cfd.de/index.php...rische-schemen

If think the new link is this one: http://www.holzmann-cfd.de/index.php/numerische-schemen

Best regards,
Bruno

Tobi · December 25, 2013, 12:03

Hi Ehsan,

here is the actual link:

http://www.holzmann-cfd.de/index.php/numerische-schemen

May 23, 2013, 08:18		#4
immortality Senior Member Ehsan Join Date: Oct 2012 Location: Iran Posts: 2,208 Rep Power: 26	thanks Tobias related to vanLeer nothing has said but it has nice results,then what do you suggest for better accurate and physical results for passive scalar transport? __________________ Injustice Anywhere is a Threat for Justice Everywhere.Martin Luther King. To Be or Not To Be,Thats the Question! The Only Stupid Question Is the One that Goes Unasked.

May 23, 2013, 14:45		#6
immortality Senior Member Ehsan Join Date: Oct 2012 Location: Iran Posts: 2,208 Rep Power: 26	thanks. vanLeer isn't a second order scheme? what do 1 0 1 refer to respectively in the scheme? __________________ Injustice Anywhere is a Threat for Justice Everywhere.Martin Luther King. To Be or Not To Be,Thats the Question! The Only Stupid Question Is the One that Goes Unasked.

May 23, 2013, 15:05		#7
Tobi Super Moderator Tobias Holzmann Join Date: Oct 2010 Location: Tussenhausen Posts: 2,708 Blog Entries: 6 Rep Power: 51	vanLeer is a second order scheme. To prevent unphysical results (the only scheme which is not producing unphysical results is gauss upwind 1st order) you can use limited schemes and schemes that are bouding the values: Code: limtiedLinear 1 limitedLinear 0.33 limitedLinear 0 = linear The number behind the name is the value of the lmiiter. If you set it to one you have full limited functionallity. If you set it to zero there is no limiting in the scheme so you have the normal linear scheme. Code: limitedLimitedLinear 1 0 1 - first number is for the limiter function as befor - the second one is the lower bouding value - the third one is the upper bouding value As you set your scalar between 0-13.54 you should write: Code: limitedLimitedLinear 1 0 13.54 immortality likes this. Last edited by Tobi; May 24, 2013 at 07:38. Reason: prefent :D

May 23, 2013, 15:21		#8
immortality Senior Member Ehsan Join Date: Oct 2012 Location: Iran Posts: 2,208 Rep Power: 26	thank you for your full clarification. __________________ Injustice Anywhere is a Threat for Justice Everywhere.Martin Luther King. To Be or Not To Be,Thats the Question! The Only Stupid Question Is the One that Goes Unasked.

May 25, 2013, 16:16		#9
immortality Senior Member Ehsan Join Date: Oct 2012 Location: Iran Posts: 2,208 Rep Power: 26	Hi again! and what will be the proper code for an incompressible case? I wrote sp(rho,gas) in pimpleFoam and it got an error and when removed rho from equation in got another error:http://www.cfd-online.com/Forums/ope...tml#post430020 so whats the correct equation? __________________ Injustice Anywhere is a Threat for Justice Everywhere.Martin Luther King. To Be or Not To Be,Thats the Question! The Only Stupid Question Is the One that Goes Unasked.

May 23, 2013, 07:21		#3
Tobi Super Moderator Tobias Holzmann Join Date: Oct 2010 Location: Tussenhausen Posts: 2,708 Blog Entries: 6 Rep Power: 51	Info about the added Lines: Sp(...) -> http://www.cfd-online.com/Forums/ope...tml#post407482

May 26, 2013, 13:18		#12
Tobi Super Moderator Tobias Holzmann Join Date: Oct 2010 Location: Tussenhausen Posts: 2,708 Blog Entries: 6 Rep Power: 51	Sorry... my fault: Code: fvm::ddt(gas)

December 25, 2013, 10:46		#14
immortality Senior Member Ehsan Join Date: Oct 2012 Location: Iran Posts: 2,208 Rep Power: 26	Hi dear Tobias this link has been broken,could you give me another link for referencing? thanks. http://www.holzmann-cfd.de/index.php...rische-schemen __________________ Injustice Anywhere is a Threat for Justice Everywhere.Martin Luther King. To Be or Not To Be,Thats the Question! The Only Stupid Question Is the One that Goes Unasked.

December 25, 2013, 12:03		#16
Tobi Super Moderator Tobias Holzmann Join Date: Oct 2010 Location: Tussenhausen Posts: 2,708 Blog Entries: 6 Rep Power: 51	Hi Ehsan, here is the actual link: http://www.holzmann-cfd.de/index.php/numerische-schemen wyldckat likes this.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
whats the cause of error?	immortality	OpenFOAM Running, Solving & CFD	13	March 24, 2021 07:15
dieselFoam problem!! trying to introduce a new heat transfer model	vivek070176	OpenFOAM Programming & Development	10	December 23, 2014 23:48
compressible flow in turbocharger	riesotto	OpenFOAM	50	May 26, 2014 01:47
is internalField(U) equivalent to zeroGradient?	immortality	OpenFOAM Running, Solving & CFD	7	March 29, 2013 01:27
passive scalar for carbon monoxide	kraizy	STAR-CCM+	0	October 12, 2009 20:13