MRFSimpleFoam implementation questions

Horus · February 15, 2013, 06:51

Hello,

I''m digging into the MRF implementation of MRFSimpleFoam.
For understanding the mathematics I've found [1] and [2].

The MRFSimpleFoam source code [3]. The rhs of the momentum equation is added a sources term for coriolis forces.
pEqn.H calls mrfZones.relativeFlux(phi); which "makes the given absolute mass/vol flux relative within the MRF region". So we are working with relative velocity, correct?

In MRFZone.C [4] Foam::MRFZone::addCoriolis(fvVectorMatrix& UEqn) is called. It adds the source term Usource[celli] -= V[celli]*(Omega ^ U[celli]); to every cell within the MRF zone.

U is relative velocity, V is the cell volume, Omega the rotating axis/frequency, ^ the cross product.

- If we're using relative velocity, doesn't the coriolis term needs to be 2 * omega ^ Urel ?
- Where is the centripetal force term omega ^ omega ^ r? Is is contained in fvm::laplacian(rAU, p) in pEqn?
- Why the cell volume? The compressible addCoriolis function uses -V * rho which is mass...

Thanks for any clarifications!

Florian

[1] http://openfoamwiki.net/index.php/Se...RF_development
[2] http://openfoamwiki.net/index.php/Si...ry_MRF_Library
[3] http://foam.sourceforge.net/docs/cpp...e79dad982.html
[4] http://foam.sourceforge.net/docs/cpp/a03948_source.html

Horus · February 22, 2013, 04:42

Dare to bump that...

chegdan · February 22, 2013, 17:25

Florian,

Glad you asked this question, it made me look at it MRF solvers a little more closely.

Quote:

- If we're using relative velocity, doesn't the coriolis term needs to be 2 * omega ^ Urel ?

The velocity in MRFSimpleFOAM is in absolute velocity, therefore the Coriolis acceleration is correctly formulated and rolled into a single term with centripetal force.

Quote:

- Where is the centripetal force term omega ^ omega ^ r? Is is contained in fvm::laplacian(rAU, p) in pEqn?

For absolute velocity, the centripetal force and coriolis force collapse into the single form

$V_{cell}(\vec{\omega}\times\vec{U})$

Quote:

Why the cell volume? The compressible addCoriolis function uses -V * rho which is mass..

The incompressible formulation of the momentum transport equation has already been divided by rho. Hence why we use nu ( mu divide by rho) and density normalized pressure (in terms of pressure divided by rho...check the units of pressure in simpleFoam cases). Therefore the multiplication of the source term by cell volume is necessary to get the units of force.

Horus · February 25, 2013, 09:09

Quote:

Originally Posted by chegdan

Florian,
The velocity in MRFSimpleFOAM is in absolute velocity, therefore the Coriolis acceleration is correctly formulated and rolled into a single term with centripetal force.

For absolute velocity, the centripetal force and coriolis force collapse into the single form

$V_{cell}(\vec{\omega}\times\vec{U})$

Thanks for your reply!

The equation used is Eqn. 6 at http://openfoamwiki.net/index.php/Se...RF_development . Correct?

There is the expression

$\nabla \cdot (\vec u_R \otimes \vec u_I)$

The dyadic product of relative and absolute velocity. I still don't really understand where this expression has gone in the source code?

Thanks!

Florian

chegdan · February 25, 2013, 11:37

Florian,

Glancing at other CFD packages documentation and the formulation for MRF solvers, I do see this term as well and seems that it would make sense that the advection term

$\nabla\cdot(\vec{U_R}\vec{U})$ ,

should in fact be in there somewhere. If the absolute velocity is the variable of interest, then U_R is related to phi and coupled explicitly through some phi adjustment.

If you look further in the MRFSimpleFoam, you will see the pEqn.H. In that file there is a method that is called that adjusts the flux for this:

Code:

mrfZones.relativeFlux(phi)

If you look into the files located in

Code:

$FOAM_SRC/finiteVolume/cfdTools/general/MRF

You will see the

Code:

relativeFlux()

method definition. Good luck and i hope this helps!

GerhardHolzinger · December 19, 2013, 10:07

I have one question regarding the unsteady term of Eq. 6 in [1]. There, the relative velocity appears in the time derivative.

Am I correct, that OpenFOAM computes the absolute velocity in all zones?

If that is the case: why is the relative velocity in the unsteady term?

Maybe one of you can elaborate.

Cheers,

[1] http://openfoamwiki.net/index.php/Se...RF_development

antoniofct · March 14, 2014, 05:58

Hi guys.
I have a question regarding MRF.

I have printed the output of UEqn.source() (meaning Usource[celli] -= V[celli]*(Omega ^ U[celli]) ) before and after adding coriolis term ( mrfzones.addCoriolis(rho, UEqn) ), and it prints the same. Why isnt the UEqn being updated??

Thanks

Ruli · March 15, 2014, 10:59

Quote:

Originally Posted by GerhardHolzinger

Am I correct, that OpenFOAM computes the absolute velocity in all zones?

Yep, that`s true

Quote:

Originally Posted by GerhardHolzinger

If that is the case: why is the relative velocity in the unsteady term?

Looking at http://openfoamwiki.net/index.php/Se...RF_development the temporal term of the 'original' NS equation is transformed into its relative formulation, which leads to U_rel in unsteady term. This term is not affected by the further simplifications. I guess it is treated explicitely.

Best regards
Julian

February 15, 2013, 06:51	MRFSimpleFoam implementation questions	#1
Horus Member Florian Join Date: Nov 2009 Posts: 59 Rep Power: 17	Hello, I''m digging into the MRF implementation of MRFSimpleFoam. For understanding the mathematics I've found [1] and [2]. The MRFSimpleFoam source code [3]. The rhs of the momentum equation is added a sources term for coriolis forces. pEqn.H calls mrfZones.relativeFlux(phi); which "makes the given absolute mass/vol flux relative within the MRF region". So we are working with relative velocity, correct? In MRFZone.C [4] Foam::MRFZone::addCoriolis(fvVectorMatrix& UEqn) is called. It adds the source term Usource[celli] -= V[celli](Omega ^ U[celli]); to every cell within the MRF zone. U is relative velocity, V is the cell volume, Omega the rotating axis/frequency, ^ the cross product. - If we're using relative velocity, doesn't the coriolis term needs to be 2 omega ^ Urel ? - Where is the centripetal force term omega ^ omega ^ r? Is is contained in fvm::laplacian(rAU, p) in pEqn? - Why the cell volume? The compressible addCoriolis function uses -V * rho which is mass... Thanks for any clarifications! Florian [1] http://openfoamwiki.net/index.php/Se...RF_development [2] http://openfoamwiki.net/index.php/Si...ry_MRF_Library [3] http://foam.sourceforge.net/docs/cpp...e79dad982.html [4] http://foam.sourceforge.net/docs/cpp/a03948_source.html

February 25, 2013, 11:37		#5
chegdan Senior Member Daniel P. Combest Join Date: Mar 2009 Location: St. Louis, USA Posts: 621 Rep Power: 0	Florian, Glancing at other CFD packages documentation and the formulation for MRF solvers, I do see this term as well and seems that it would make sense that the advection term $\nabla\cdot(\vec{U_R}\vec{U})$ , should in fact be in there somewhere. If the absolute velocity is the variable of interest, then U_R is related to phi and coupled explicitly through some phi adjustment. If you look further in the MRFSimpleFoam, you will see the pEqn.H. In that file there is a method that is called that adjusts the flux for this: Code: mrfZones.relativeFlux(phi) If you look into the files located in Code: $FOAM_SRC/finiteVolume/cfdTools/general/MRF You will see the Code: relativeFlux() method definition. Good luck and i hope this helps!

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Wall functions - questions about implementation	AlmostSurelyRob	OpenFOAM Programming & Development	44	May 6, 2020 11:11
MRFSimpleFoam Tutorial	bastil	OpenFOAM Running, Solving & CFD	48	August 1, 2012 11:00
GGI implementation in MRFSimpleFoam	amgode	OpenFOAM Running, Solving & CFD	8	August 5, 2011 07:03
about MRFSimpleFoam and ggi	wllmk1	OpenFOAM Running, Solving & CFD	0	February 5, 2011 05:52
Implementation issues of fvSchemes / laplacianScheme, in particular gaussLaplacianSch	thomek	OpenFOAM Programming & Development	0	October 18, 2010 06:10

February 22, 2013, 04:42		#2
Horus Member Florian Join Date: Nov 2009 Posts: 59 Rep Power: 17	Dare to bump that...

December 19, 2013, 10:07		#6
GerhardHolzinger Senior Member Gerhard Holzinger Join Date: Feb 2012 Location: Austria Posts: 342 Rep Power: 28	I have one question regarding the unsteady term of Eq. 6 in [1]. There, the relative velocity appears in the time derivative. Am I correct, that OpenFOAM computes the absolute velocity in all zones? If that is the case: why is the relative velocity in the unsteady term? Maybe one of you can elaborate. Cheers, [1] http://openfoamwiki.net/index.php/Se...RF_development

March 14, 2014, 05:58		#7
antoniofct New Member Join Date: Oct 2011 Posts: 27 Rep Power: 15	Hi guys. I have a question regarding MRF. I have printed the output of UEqn.source() (meaning Usource[celli] -= V[celli]*(Omega ^ U[celli]) ) before and after adding coriolis term ( mrfzones.addCoriolis(rho, UEqn) ), and it prints the same. Why isnt the UEqn being updated?? Thanks