calculation of phi

wbetz · August 21, 2009, 09:44

Where do I have to look (in the source code), if I want to know how phi is calculated in interFoam?

l_r_mcglashan · August 22, 2009, 06:16

In createFields.H, you'll see the line include "createPhi.H". You can find this in OpenFOAM-1.X/src/finiteVolume/cfdTools/incompressible

It is defined as:

phi = linearInterpolate(U) & mesh.Sf()

I think the best thing to do is to set up your IDE's code assistance, so that you can easily navigate through the source code.

wbetz · August 22, 2009, 07:02

If phi is calculated from U, what is the advantage of using boundary conditions like fluxCorrectedVelocity, pressureInletVelocity, pressureInletOutletVelocity - which calculate U form the flux(phi)?

l_r_mcglashan · August 22, 2009, 07:35

I've had a quick look at fluxCorrectedVelocity.
It would be used when you know the pressure at a boundary and the flux through that boundary.
The BC is correcting the velocity component normal to the boundary, based on your knowledge of the flux through that boundary.
I can't think of when I would use it, maybe someone else has?

You could replace all instances of phi with linearInterpolate(U) & mesh.Sf(), but that would make the code messy.

belier1988 · November 7, 2018, 10:21

Quote:

Originally Posted by wbetz

If phi is calculated from U, what is the advantage of using boundary conditions like fluxCorrectedVelocity, pressureInletVelocity, pressureInletOutletVelocity - which calculate U form the flux(phi)?

This is a very interesting question. I'v wondered about it during the use of pimpleFoam with the BC types such as pressureInletVelocity. My guess is that at the boundary where pressure is known, phi is calculated from pressure and can be used to give a value to the velocity component normal to the path.
Can anyone provide a better answer to clear things up ?

Tobi · November 8, 2018, 01:16

Hi all,

this is an ancient thread, but I want to give some hints:

The flux phi is estimated by the velocity rho*U (compressible) or U (incompressible)
However, the flux itself is corrected using the pressure equation, and then, the new velocity is recalculated from the fluxes
So you cannot say, phi is estimated from U, and after that, it is similar to estimate U from the flux phi because of the flux change during the pressure equation.

Lets consider the solver pimpleFoam

At the beginning the flux field is created in createPhi.H while the values are calculated from U; this is an initialization guess (https://github.com/OpenFOAM/OpenFOAM...teFields.H#L29)
Inside the pimple-loop we have several things that change the flux field such as moving meshes, multi-reference frame and so on (I don´t consider that now).
Neglecting the modifications to the phi field based on the above-mentioned functionalities, we go into the UEqn.H (https://github.com/OpenFOAM/OpenFOAM...pleFoam/UEqn.H)
Here we do not modify the flux field; we construct the momentum matrix, and if the momentum predictor is on, we estimate a new velocity field based on Navier Stokes equation (not required in general).
After that we enter to the pEqn.H. Inside the pressure loop, we update the fluxes according to the new pressure field (https://github.com/OpenFOAM/OpenFOAM...oam/pEqn.H#L51)
After the pressure is calculated, it is evident that the fluxes are different to the corresponding velocities field (still the old one), that´s why we need to recalculate the new velocity field from the new fluxes (https://github.com/OpenFOAM/OpenFOAM...oam/pEqn.H#L60)
After correcting the internal domain, we adjust the boundary conditions for U (https://github.com/OpenFOAM/OpenFOAM...oam/pEqn.H#L61)

Now it should be clear, that the flux-corrected boundary conditions are useful because the fluxes are changing during the pressure equation and we recalculate the velocity from the new fluxes.

belier1988 · November 14, 2018, 05:06

Thanks Tobi, it's more clear for me now. Have a nice day.

Bdew8556 · May 28, 2019, 20:04

Hey guys.

I know it's meant to be poor form, but this is directly relevant.
Any thoughts??

Flow rate and phi not matching??

Diro7 · December 29, 2020, 05:52

Hello guys,

thanks for the brilliant material.
I have a related question:

Suppose that I have to solve an additional transport equation for a velocity field V (which is not the standard velocity field U, but may depend on it).
I understand that I have to define a new flux field (no problem to create it), but how should I ensure a correct treatment of flux and velocity provided that they don't need to satisfy a coupled pressure equation?

Things should be necessarily easier than in the standard U-p coupling, but I don't understand clearly what bits should I retain from a standard (S,P)IMPLE solver.

For reference, the transport equation for

reads like

$\frac{\partial (c V_i)}{\partial t} + \frac{\partial (c V_i V_k)}{\partial x_k} = c F_i$

where repeated index summation notation is assumed and

is a "concentration or density" field which satisfies a transport equation of the form

$\frac{\partial c}{\partial t} + \frac{\partial (c V_k)}{\partial x_k} = \frac{\partial}{\partial x_k} \left( D \frac{\partial c}{\partial x_k} \right)$

The two equations can be implemented rather straightforwardly provided that a new correct flux $\phi_c$ is used. Upon creation it can be defined by interpolation like in a compressible solver, but how should I ensure the correct update of $\phi_c$ like it is done in a pEqn.H?

Thanks in advance to everyone who has some advice

August 21, 2009, 09:44	calculation of phi	#1
wbetz New Member Wolfgang Betz Join Date: Mar 2009 Posts: 6 Rep Power: 17	Where do I have to look (in the source code), if I want to know how phi is calculated in interFoam?

August 22, 2009, 06:16		#2
l_r_mcglashan Senior Member Laurence R. McGlashan Join Date: Mar 2009 Posts: 370 Rep Power: 23	In createFields.H, you'll see the line include "createPhi.H". You can find this in OpenFOAM-1.X/src/finiteVolume/cfdTools/incompressible It is defined as: phi = linearInterpolate(U) & mesh.Sf() I think the best thing to do is to set up your IDE's code assistance, so that you can easily navigate through the source code. allanZHONG likes this. __________________ Laurence R. McGlashan :: Website

August 22, 2009, 07:35		#4
l_r_mcglashan Senior Member Laurence R. McGlashan Join Date: Mar 2009 Posts: 370 Rep Power: 23	I've had a quick look at fluxCorrectedVelocity. It would be used when you know the pressure at a boundary and the flux through that boundary. The BC is correcting the velocity component normal to the boundary, based on your knowledge of the flux through that boundary. I can't think of when I would use it, maybe someone else has? You could replace all instances of phi with linearInterpolate(U) & mesh.Sf(), but that would make the code messy. __________________ Laurence R. McGlashan :: Website

November 8, 2018, 01:16		#6
Tobi Super Moderator Tobias Holzmann Join Date: Oct 2010 Location: Tussenhausen Posts: 2,708 Blog Entries: 6 Rep Power: 51	Hi all, this is an ancient thread, but I want to give some hints: The flux phi is estimated by the velocity rhoU (compressible) or U (incompressible) However, the flux itself is corrected using the pressure equation, and then, the new velocity is recalculated from the fluxes So you cannot say, phi is estimated from U, and after that, it is similar to estimate U from the flux phi because of the flux change during the pressure equation. Lets consider the solver pimpleFoam* At the beginning the flux field is created in createPhi.H while the values are calculated from U; this is an initialization guess (https://github.com/OpenFOAM/OpenFOAM...teFields.H#L29) Inside the pimple-loop we have several things that change the flux field such as moving meshes, multi-reference frame and so on (I don´t consider that now). Neglecting the modifications to the phi field based on the above-mentioned functionalities, we go into the UEqn.H (https://github.com/OpenFOAM/OpenFOAM...pleFoam/UEqn.H) Here we do not modify the flux field; we construct the momentum matrix, and if the momentum predictor is on, we estimate a new velocity field based on Navier Stokes equation (not required in general). After that we enter to the pEqn.H. Inside the pressure loop, we update the fluxes according to the new pressure field (https://github.com/OpenFOAM/OpenFOAM...oam/pEqn.H#L51) After the pressure is calculated, it is evident that the fluxes are different to the corresponding velocities field (still the old one), that´s why we need to recalculate the new velocity field from the new fluxes (https://github.com/OpenFOAM/OpenFOAM...oam/pEqn.H#L60) After correcting the internal domain, we adjust the boundary conditions for U (https://github.com/OpenFOAM/OpenFOAM...oam/pEqn.H#L61) Now it should be clear, that the flux-corrected boundary conditions are useful because the fluxes are changing during the pressure equation and we recalculate the velocity from the new fluxes. snak, lth, nishant.kumar and 7 others like this. __________________ Keep foaming, Tobias Holzmann

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Turbulence Model phi vs phi_	doug	OpenFOAM Running, Solving & CFD	4	November 10, 2009 04:33
Another phi question	ehsan_vaghefi	OpenFOAM Running, Solving & CFD	0	October 24, 2008 19:56
Calculation of phi if velocity field is known	ankgupta8um	OpenFOAM Running, Solving & CFD	5	October 15, 2006 03:46
Warning 097-	AB	Siemens	6	November 15, 2004 04:41
Heat Flux Calculation under REPORTS	Alberto Schroth	FLUENT	0	May 16, 2000 08:19

August 22, 2009, 07:02		#3
wbetz New Member Wolfgang Betz Join Date: Mar 2009 Posts: 6 Rep Power: 17	If phi is calculated from U, what is the advantage of using boundary conditions like fluxCorrectedVelocity, pressureInletVelocity, pressureInletOutletVelocity - which calculate U form the flux(phi)?

November 14, 2018, 05:06		#7
belier1988 New Member ghuang Join Date: Oct 2014 Posts: 3 Rep Power: 11	Thanks Tobi, it's more clear for me now. Have a nice day.

May 28, 2019, 20:04		#8
Bdew8556 Senior Member Brett Join Date: May 2013 Posts: 212 Rep Power: 13	Hey guys. I know it's meant to be poor form, but this is directly relevant. Any thoughts?? Flow rate and phi not matching??

December 29, 2020, 05:52		#9
Diro7 Member Andrea Di Ronco Join Date: Nov 2016 Location: Milano, Italy Posts: 57 Rep Power: 9	Hello guys, thanks for the brilliant material. I have a related question: Suppose that I have to solve an additional transport equation for a velocity field V (which is not the standard velocity field U, but may depend on it). I understand that I have to define a new flux field (no problem to create it), but how should I ensure a correct treatment of flux and velocity provided that they don't need to satisfy a coupled pressure equation? Things should be necessarily easier than in the standard U-p coupling, but I don't understand clearly what bits should I retain from a standard (S,P)IMPLE solver. For reference, the transport equation for reads like $\frac{\partial (c V_i)}{\partial t} + \frac{\partial (c V_i V_k)}{\partial x_k} = c F_i$ where repeated index summation notation is assumed and is a "concentration or density" field which satisfies a transport equation of the form $\frac{\partial c}{\partial t} + \frac{\partial (c V_k)}{\partial x_k} = \frac{\partial}{\partial x_k} \left( D \frac{\partial c}{\partial x_k} \right)$ The two equations can be implemented rather straightforwardly provided that a new correct flux $\phi_c$ is used. Upon creation it can be defined by interpolation like in a compressible solver, but how should I ensure the correct update of $\phi_c$ like it is done in a pEqn.H? Thanks in advance to everyone who has some advice