I need explanations about fixedFluxPressure

Cyp · November 30, 2010, 04:15

Hello!

I had a look at the fixedFluxPressure boundary condition and I am not quite sure to well understand what this BC does.

I guess I have to use this BC if I want to evaluate the pressure according to a velocity input. Am I wrong ?

Furthermore, in the code source, one can read:

Code:

        gradient() = (phip - (patch().Sf() & Up))/patch().magSf()/rAp;

I do not succeed in linking this snippet with a mathematical formula...

All enlightments are welcome!
Regards,
Cyp

JR22 · August 19, 2013, 20:36

I realize this is an old thread, but it is still very relevant.

I was having terrible problems trying to get buoyantBoussinesqSimpleFoam to converge. I changed the p_rgh BC's from buoyantPressure to fixedFluxPressure and the model started to converge.

Anybody?

Sherlock_1812 · August 1, 2014, 04:42

Same question here. What is the difference between buoyantPressure and fixedFLuxPressure boundary conditions?

zandi · October 16, 2014, 02:23

Hi
OpenFAOM version 2.3.0 doesn't have buoyantPressure libraries. Am I right?
what is the difference between buoyantPressure and fixedFluxPressure?
why fixedFluxPressure converge better? is it the only difference between them?
Please help

fabian_roesler · October 16, 2014, 03:46

OpenFOAM 2.2.2 has both boundary conditions. In newer Version, buoyantPressure boundary was dismissed. For clarification have a look into the code or into Doxygen.

From buoyantPressureFvPatchScalarField we learn that:
This boundary condition sets the pressure gradient appropriately for buoyant flow. If the variable name is one of pd, p_rgh or ph_rgh, we assume that the pressure variable is $p - \rho(g \cdot h)$ and the gradient set using:
$\nabla(p) = -\nabla_\perp(\rho)(g \cdot h)$
Otherwise we assume that it is the static pressure, and the gradient calculated using:
$\nabla(p) = \rho(g \cdot n)$

From fixedFluxPressureFvPatchScalarField we see that:
This boundary condition adjusts the pressure gradient such that the flux on the boundary is that specified by the velocity boundary condition.
The predicted flux to be compensated by the pressure gradient is evaluated as $$(\phi - \phi_{H/A})$ , both of which are looked-up from the database, as is the pressure diffusivity used to calculate the gradient using:
$\nabla(p) = \frac{\phi_{H/A} - \phi}{|Sf| D_p}$

fabian_roesler · October 16, 2014, 04:21

Some additional remarks:

The fixedFluxPressure boundary is known do have a better convergence. This is in my opinion due to the more pressure related calculation of the gradient:
$\nabla(p) = \frac{\phi_{H/A} - \phi}{|Sf| D_p}$
phi and phiHbyA (predicted flux field) are directly linked to pressure equation. On a wall, the flux difference tends to zero and so the boundary condition turns to zeroGradient.
The buoyanPressure boundary is more the physical method to describe the pressure gradient with Archimedes' principle.
I hope my explanation is understandable and correct.

Cheers

Fabian

santiagomarquezd · November 5, 2014, 16:06

Hi folks, I'm dealing with fixedFluxPressure BCs also and this thread was helpful. Checking the code things have changed at least in FOAM 2.3.0. The class definition is now more simple

fixedFluxPressureFvPatchScalarField.C

Code:

  125 void Foam::fixedFluxPressureFvPatchScalarField::updateCoeffs
  126 (
  127     const scalarField& snGradp
  128 )
  129 {
  130     if (updated())
  131     {
  132         return;
  133     }
  134 
  135     curTimeIndex_ = this->db().time().timeIndex();
  136 
  137     gradient() = snGradp;
  138     fixedGradientFvPatchScalarField::updateCoeffs();
  139 }

it only sets the proper gradient in line 137 and then calls the updateCoeffs() method from the fixedGradientFvPatchScalarField class (from which the present class inherits). This requires to set the value of snGradp which is done at solver level. For example, from pEqn.H of interFoam we have:

Code:

   27     // Update the fixedFluxPressure BCs to ensure flux consistency
   28     setSnGrad<fixedFluxPressureFvPatchScalarField>
   29     (
   30         p_rgh.boundaryField(),
   31         (
   32             phiHbyA.boundaryField()
   33           - (mesh.Sf().boundaryField() & U.boundaryField())
   34         )/(mesh.magSf().boundaryField()*rAUf.boundaryField())
   35     );

From the new code the gradient reads:

$\vec{\nabla}p = \left(\vec{H}/a_P\cdot\vec{S}_f - \vec{U}\cdot\vec{S}_f\right)\frac{(a_P)_f}{||\vec{S}_f||}$

Hope this helps for 2.3.0 users.

Regards.

ssss · April 14, 2015, 16:46

I would like to comment out a bit, why does OpenFOAM use the expression given by santiagomarquezd (gracias por el análisis del código fuente) for the pressure surface normal gradient in the boundaries.

First of all we need to write down the momentum equation discretized using the Rhie-Chow interpolation method. This reads:

$\vec{u}_f = \left( \dfrac{\vec{h}}{a_p}\right)_f - \left( \dfrac{1}{a_p}\right)_f \nabla p_m$

Where the f subscript means interpolate to the face,

is the variable p_rgh whose value is $p_m=p-\rho \vec{g} \cdot \vec{h}$ , and the vector u is the velocity. Now multiply the equation by the face surface vector $\vec{S}_f = ||S_f|| \cdot \vec{n}$ where the vector n is the surface normal:

$\vec{u}_f \cdot \vec{S}_f = \left( \dfrac{\vec{h}}{a_p}\right)_f \cdot \vec{S}_f - \left( \dfrac{1}{a_p}\right)_f \nabla p_m \cdot \vec{S_f}$

Thus the following equation for the pressure surface gradient $\nabla p_m \cdot \vec{n}$ can be obtained:

$\nabla p_m \cdot \vec{n} =\left ( \left( \dfrac{\vec{h}}{a_p}\right)_f \cdot \vec{S}_f - \vec{u}_f \cdot \vec{S}_f \right) \dfrac{a_p|_f}{||S_f||}$

Hope this is useful for you foamers

angelmonsalve · October 14, 2015, 13:55

Thanks for the explanation!!

JonW · August 31, 2016, 14:35

Dear all, thank you for the above discussion

There is one thing I don't understand fully. In the damBreak example for interFoam (say of OF 4.0) the b.c. for p_rgh is given as...

leftWall
{
type fixedFluxPressure;
value uniform 0;
}

so the question is, what does "value uniform 0;" stand for?

There is one constructor in fixedFluxPressureFvPatchScalarField.C which has 3 arguments:
Foam::fixedFluxPressureFvPatchScalarField::fixedFl uxPressureFvPatchScalarField
(
const fvPatch& p,
const DimensionedField<scalar, volMesh>& iF,
const dictionary& dict
)
... and in that function body, there is
if (dict.found("value") && dict.found("gradient"))

But in interFoam, this constructor is not used, since it is the constructor with two arguments that is used (actually the first constructor), c.f. in pEqn.H

setSnGrad<fixedFluxPressureFvPatchScalarField>
(
p_rgh.boundaryField(),
(
phiHbyA.boundaryField()
- fvOptions.relative(mesh.Sf().boundaryField() & U.boundaryField())
)/(mesh.magSf().boundaryField()*rAUf.boundaryField() )
);

So am I understanding this correctly: When using interFoam, then the "value uniform 0;" is actually not used?

Any comment would be helpful
J.

decah · November 23, 2016, 17:45

Hi Jon,

I had a similar question about flowRateInletVelocity which requires an input value that doesn't appear to do anything. As explained by Roman in the below thread some derived boundary conditions necessarily inherit a placeholder value like this one because of their basic structure.

http://www.cfd-online.com/Forums/ope...tvelocity.html

I think the value uniform 0; you asked about is like this and could be assigned any value you like without affecting your simulation.

nw_ds · January 18, 2017, 04:46

So the bottom line, The difference between this bc and zeroGradient is in term of the convergence (HOW MANY ITER TO SOLVE THE PRESSURE EQN ) not the accuracy or whether the solver will converge or not.

beh_zadi · October 11, 2017, 11:22

Hi openfoam users,

I'm new to openfoam and I need your help about fixedFluxPressure BC. I have made a new solver derived from icoFoam and I didn't find the following code in it while it exists in interFoam.
I specified fixedValue BC for velocity field and fixedFluxPressure for pressure field. Does it need to add the following code in new solver to ensure flux consistency or not?

Code:

   
   27     // Update the fixedFluxPressure BCs to ensure flux consistency
   28     setSnGrad<fixedFluxPressureFvPatchScalarField>
   29     (
   30         p_rgh.boundaryField(),
   31         (
   32             phiHbyA.boundaryField()
   33           - (mesh.Sf().boundaryField() & U.boundaryField())
   34         )/(mesh.magSf().boundaryField()*rAUf.boundaryField())
   35     );

Any comment would be helpful

roenby · December 14, 2017, 08:58

Just for the record:

If you are using a newer version of OpenFOAM (e.g. 5.x), you will find that the referred code snippet from interFoam's pEqn.H file has been replaced by the function call:

constrainPressure(p_rgh, U, phiHbyA, rAUf, MRF);

This is also the case for icoFoam.

In the source code for this function, you'll find a similar code snippet:

https://github.com/OpenFOAM/OpenFOAM...Pressure.C#L34

Best,
Johan

Andrea1984 · April 30, 2020, 08:21

Apologies for digging up and old thread.

I have noticed that the call to constrainPressure does not take place in the Eulerian multiphase solvers (I am using OpenFOAM 6.0). I take this means that zeroGradient and fixedFluxPressure are equivalent for this class of solvers. Would be useful is some can confirm this.

Cheers,
Andrea

Andrea1984 · April 30, 2020, 09:00

Ok so to answer my previous question, in multiphase Eulerian solvers this is done within pEqn without calling the constrainPressure function (probably because this is only suitable for one-fluid solvers).

In twoPhaseEulerFoam's pEqn.H this is done by

Code:

    // Update the fixedFluxPressure BCs to ensure flux consistency
    setSnGrad<fixedFluxPressureFvPatchScalarField>
    (
        p_rgh.boundaryFieldRef(),
        (
            phiHbyA.boundaryField()
          - (
                alphaf1.boundaryField()*phi1.boundaryField()
              + alphaf2.boundaryField()*phi2.boundaryField()
            )
        )/(mesh.magSf().boundaryField()*rAUf.boundaryField())
    );

The same is done in the pressure equation of the reactingEulerFoam family.
So to conclude the answer to my question in the previous post is no: fixedFluxPressure and zeroGradient are NOT the same thing in multiphase Eulerian solvers.

Mars409 · May 27, 2022, 10:01

All that updateCoeffs() does, as defined in fvPatchField.C, is setting flag update_ to true:

Code:

template<class Type>
 void Foam::fvPatchField<Type>::updateCoeffs()
 {
     updated_ = true;
 }

Mars409 · May 28, 2022, 11:01

The fixedFluxPressure boundary condition and the constrainPressure() function are now explained in a detailed openFOAM Wiki article on the SimpleFOAM solver:

https://openfoamwiki.net/index.php/S...ssure_equation

November 30, 2010, 04:15	I need explanations about fixedFluxPressure	#1
Cyp Senior Member Cyprien Join Date: Feb 2010 Location: Stanford University Posts: 299 Rep Power: 18	Hello! I had a look at the fixedFluxPressure boundary condition and I am not quite sure to well understand what this BC does. I guess I have to use this BC if I want to evaluate the pressure according to a velocity input. Am I wrong ? Furthermore, in the code source, one can read: Code: gradient() = (phip - (patch().Sf() & Up))/patch().magSf()/rAp; I do not succeed in linking this snippet with a mathematical formula... All enlightments are welcome! Regards, Cyp JR22, Guimloute, amuzeshi and 1 others like this.

August 19, 2013, 20:36	buoyantPressure vs. fixedFluxPressure	#2
JR22 Senior Member Jose Rey Join Date: Oct 2012 Posts: 134 Rep Power: 17	I realize this is an old thread, but it is still very relevant. I was having terrible problems trying to get buoyantBoussinesqSimpleFoam to converge. I changed the p_rgh BC's from buoyantPressure to fixedFluxPressure and the model started to converge. Anybody? Guimloute and amuzeshi like this.

August 1, 2014, 04:42		#3
Sherlock_1812 Senior Member Srivathsan N Join Date: Jan 2013 Location: India Posts: 101 Rep Power: 13	Same question here. What is the difference between buoyantPressure and fixedFLuxPressure boundary conditions? __________________ Regards, Srivaths

October 16, 2014, 02:23	OpenFAOM 2.3.0 doesn't have buoyantPressure BC	#4
zandi Senior Member Fatema Zandi Goharrizi Join Date: Mar 2009 Posts: 158 Rep Power: 17	Hi OpenFAOM version 2.3.0 doesn't have buoyantPressure libraries. Am I right? what is the difference between buoyantPressure and fixedFluxPressure? why fixedFluxPressure converge better? is it the only difference between them? Please help

October 16, 2014, 03:46		#5
fabian_roesler Senior Member Fabian Roesler Join Date: Mar 2009 Location: Germany Posts: 213 Rep Power: 18	OpenFOAM 2.2.2 has both boundary conditions. In newer Version, buoyantPressure boundary was dismissed. For clarification have a look into the code or into Doxygen. From buoyantPressureFvPatchScalarField we learn that: This boundary condition sets the pressure gradient appropriately for buoyant flow. If the variable name is one of pd, p_rgh or ph_rgh, we assume that the pressure variable is $p - \rho(g \cdot h)$ and the gradient set using: $\nabla(p) = -\nabla_\perp(\rho)(g \cdot h)$ Otherwise we assume that it is the static pressure, and the gradient calculated using: $\nabla(p) = \rho(g \cdot n)$ From fixedFluxPressureFvPatchScalarField we see that: This boundary condition adjusts the pressure gradient such that the flux on the boundary is that specified by the velocity boundary condition. The predicted flux to be compensated by the pressure gradient is evaluated as $$(\phi - \phi_{H/A})$ , both of which are looked-up from the database, as is the pressure diffusivity used to calculate the gradient using: $\nabla(p) = \frac{\phi_{H/A} - \phi}{\|Sf\| D_p}$ haghajani, wyldckat, zandi and 35 others like this.

October 16, 2014, 04:21		#6
fabian_roesler Senior Member Fabian Roesler Join Date: Mar 2009 Location: Germany Posts: 213 Rep Power: 18	Some additional remarks: The fixedFluxPressure boundary is known do have a better convergence. This is in my opinion due to the more pressure related calculation of the gradient: $\nabla(p) = \frac{\phi_{H/A} - \phi}{\|Sf\| D_p}$ phi and phiHbyA (predicted flux field) are directly linked to pressure equation. On a wall, the flux difference tends to zero and so the boundary condition turns to zeroGradient. The buoyanPressure boundary is more the physical method to describe the pressure gradient with Archimedes' principle. I hope my explanation is understandable and correct. Cheers Fabian haghajani, wyldckat, zandi and 33 others like this.

November 5, 2014, 16:06		#7
santiagomarquezd Senior Member Santiago Marquez Damian Join Date: Aug 2009 Location: Santa Fe, Santa Fe, Argentina Posts: 452 Rep Power: 23	Hi folks, I'm dealing with fixedFluxPressure BCs also and this thread was helpful. Checking the code things have changed at least in FOAM 2.3.0. The class definition is now more simple fixedFluxPressureFvPatchScalarField.C Code: 125 void Foam::fixedFluxPressureFvPatchScalarField::updateCoeffs 126 ( 127 const scalarField& snGradp 128 ) 129 { 130 if (updated()) 131 { 132 return; 133 } 134 135 curTimeIndex_ = this->db().time().timeIndex(); 136 137 gradient() = snGradp; 138 fixedGradientFvPatchScalarField::updateCoeffs(); 139 } it only sets the proper gradient in line 137 and then calls the updateCoeffs() method from the fixedGradientFvPatchScalarField class (from which the present class inherits). This requires to set the value of snGradp which is done at solver level. For example, from pEqn.H of interFoam we have: Code: 27 // Update the fixedFluxPressure BCs to ensure flux consistency 28 setSnGrad<fixedFluxPressureFvPatchScalarField> 29 ( 30 p_rgh.boundaryField(), 31 ( 32 phiHbyA.boundaryField() 33 - (mesh.Sf().boundaryField() & U.boundaryField()) 34 )/(mesh.magSf().boundaryField()rAUf.boundaryField()) 35 ); From the new code the gradient reads: $\vec{\nabla}p = \left(\vec{H}/a_P\cdot\vec{S}_f - \vec{U}\cdot\vec{S}_f\right)\frac{(a_P)_f}{\|\|\vec{S}_f\|\|}$ Hope this helps for 2.3.0 users. Regards. wikstrom, fabian_roesler, haghajani and 29 others like this. __________________ Santiago MÁRQUEZ DAMIÁN, Ph.D. Research Scientist Research Center for Computational Methods (CIMEC) - CONICET/UNL Tel: 54-342-4511594 Int. 7032 Colectora Ruta Nac. 168 / Paraje El Pozo (3000) Santa Fe - Argentina. http://www.cimec.org.ar Last edited by santiagomarquezd; November 7, 2014 at 05:25. Reason: Add equation*

April 14, 2015, 16:46		#8
ssss Senior Member anonymous Join Date: Aug 2014 Posts: 205 Rep Power: 12	I would like to comment out a bit, why does OpenFOAM use the expression given by santiagomarquezd (gracias por el análisis del código fuente) for the pressure surface normal gradient in the boundaries. First of all we need to write down the momentum equation discretized using the Rhie-Chow interpolation method. This reads: $\vec{u}_f = \left( \dfrac{\vec{h}}{a_p}\right)_f - \left( \dfrac{1}{a_p}\right)_f \nabla p_m$ Where the f subscript means interpolate to the face, is the variable p_rgh whose value is $p_m=p-\rho \vec{g} \cdot \vec{h}$ , and the vector u is the velocity. Now multiply the equation by the face surface vector $\vec{S}_f = \|\|S_f\|\| \cdot \vec{n}$ where the vector n is the surface normal: $\vec{u}_f \cdot \vec{S}_f = \left( \dfrac{\vec{h}}{a_p}\right)_f \cdot \vec{S}_f - \left( \dfrac{1}{a_p}\right)_f \nabla p_m \cdot \vec{S_f}$ Thus the following equation for the pressure surface gradient $\nabla p_m \cdot \vec{n}$ can be obtained: $\nabla p_m \cdot \vec{n} =\left ( \left( \dfrac{\vec{h}}{a_p}\right)_f \cdot \vec{S}_f - \vec{u}_f \cdot \vec{S}_f \right) \dfrac{a_p\|_f}{\|\|S_f\|\|}$ Hope this is useful for you foamers wikstrom, haghajani, zandi and 32 others like this.

October 14, 2015, 13:55		#9
angelmonsalve New Member Angel Monsalve Join Date: Oct 2009 Posts: 7 Rep Power: 16	Thanks for the explanation!!

August 31, 2016, 14:35	value uniform 0;	#10
JonW Senior Member Jon Elvar Wallevik Join Date: Nov 2010 Location: Reykjavik, ICELAND Posts: 103 Rep Power: 19	Dear all, thank you for the above discussion There is one thing I don't understand fully. In the damBreak example for interFoam (say of OF 4.0) the b.c. for p_rgh is given as... leftWall { type fixedFluxPressure; value uniform 0; } so the question is, what does "value uniform 0;" stand for? There is one constructor in fixedFluxPressureFvPatchScalarField.C which has 3 arguments: Foam::fixedFluxPressureFvPatchScalarField::fixedFl uxPressureFvPatchScalarField ( const fvPatch& p, const DimensionedField<scalar, volMesh>& iF, const dictionary& dict ) ... and in that function body, there is if (dict.found("value") && dict.found("gradient")) But in interFoam, this constructor is not used, since it is the constructor with two arguments that is used (actually the first constructor), c.f. in pEqn.H setSnGrad<fixedFluxPressureFvPatchScalarField> ( p_rgh.boundaryField(), ( phiHbyA.boundaryField() - fvOptions.relative(mesh.Sf().boundaryField() & U.boundaryField()) )/(mesh.magSf().boundaryField()*rAUf.boundaryField() ) ); So am I understanding this correctly: When using interFoam, then the "value uniform 0;" is actually not used? Any comment would be helpful J.

November 23, 2016, 17:45		#11
decah Member Declan Join Date: Oct 2016 Location: Ireland Posts: 40 Rep Power: 9	Hi Jon, I had a similar question about flowRateInletVelocity which requires an input value that doesn't appear to do anything. As explained by Roman in the below thread some derived boundary conditions necessarily inherit a placeholder value like this one because of their basic structure. http://www.cfd-online.com/Forums/ope...tvelocity.html I think the value uniform 0; you asked about is like this and could be assigned any value you like without affecting your simulation. JonW, amolrajan, mizzou and 3 others like this.

January 18, 2017, 04:46		#12
nw_ds New Member Mido Join Date: Mar 2011 Posts: 25 Rep Power: 15	So the bottom line, The difference between this bc and zeroGradient is in term of the convergence (HOW MANY ITER TO SOLVE THE PRESSURE EQN ) not the accuracy or whether the solver will converge or not.

October 11, 2017, 11:22		#13
beh_zadi New Member Join Date: Jan 2016 Posts: 3 Rep Power: 10	Hi openfoam users, I'm new to openfoam and I need your help about fixedFluxPressure BC. I have made a new solver derived from icoFoam and I didn't find the following code in it while it exists in interFoam. I specified fixedValue BC for velocity field and fixedFluxPressure for pressure field. Does it need to add the following code in new solver to ensure flux consistency or not? Code: 27 // Update the fixedFluxPressure BCs to ensure flux consistency 28 setSnGrad<fixedFluxPressureFvPatchScalarField> 29 ( 30 p_rgh.boundaryField(), 31 ( 32 phiHbyA.boundaryField() 33 - (mesh.Sf().boundaryField() & U.boundaryField()) 34 )/(mesh.magSf().boundaryField()*rAUf.boundaryField()) 35 ); Any comment would be helpful

December 14, 2017, 08:58		#14
roenby Member Johan Roenby Join Date: May 2011 Location: Denmark Posts: 92 Rep Power: 20	Just for the record: If you are using a newer version of OpenFOAM (e.g. 5.x), you will find that the referred code snippet from interFoam's pEqn.H file has been replaced by the function call: constrainPressure(p_rgh, U, phiHbyA, rAUf, MRF); This is also the case for icoFoam. In the source code for this function, you'll find a similar code snippet: https://github.com/OpenFOAM/OpenFOAM...Pressure.C#L34 Best, Johan Andrea1984, tiam, amolrajan and 5 others like this.

April 30, 2020, 08:21		#15
Andrea1984 Senior Member Andrea Join Date: Feb 2012 Location: Leeds, UK Posts: 179 Rep Power: 16	Apologies for digging up and old thread. I have noticed that the call to constrainPressure does not take place in the Eulerian multiphase solvers (I am using OpenFOAM 6.0). I take this means that zeroGradient and fixedFluxPressure are equivalent for this class of solvers. Would be useful is some can confirm this. Cheers, Andrea

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Rotating objects	Marcus Gellert (Gellert)	OpenFOAM Running, Solving & CFD	17	December 14, 2010 15:06
muSgsWallFunctionFvPatchField, explanations or bug ?	fgal	OpenFOAM Bugs	0	July 22, 2010 14:19
FixedFluxPressure cannot find field 1%7cAU	anger	OpenFOAM Running, Solving & CFD	3	November 10, 2008 05:50
New to CFX-need explanations about mesh parameters	Cyril	CFX	3	November 24, 2006 06:33
Rotor/stator tutorial, and how to...	gilberto	CFX	5	January 21, 2002 09:41

April 30, 2020, 09:00		#16
Andrea1984 Senior Member Andrea Join Date: Feb 2012 Location: Leeds, UK Posts: 179 Rep Power: 16	Ok so to answer my previous question, in multiphase Eulerian solvers this is done within pEqn without calling the constrainPressure function (probably because this is only suitable for one-fluid solvers). In twoPhaseEulerFoam's pEqn.H this is done by Code: // Update the fixedFluxPressure BCs to ensure flux consistency setSnGrad<fixedFluxPressureFvPatchScalarField> ( p_rgh.boundaryFieldRef(), ( phiHbyA.boundaryField() - ( alphaf1.boundaryField()phi1.boundaryField() + alphaf2.boundaryField()phi2.boundaryField() ) )/(mesh.magSf().boundaryField()*rAUf.boundaryField()) ); The same is done in the pressure equation of the reactingEulerFoam family. So to conclude the answer to my question in the previous post is no: fixedFluxPressure and zeroGradient are NOT the same thing in multiphase Eulerian solvers. granzer and Mars409 like this.

May 27, 2022, 10:01		#17
Mars409 New Member Join Date: May 2020 Posts: 29 Blog Entries: 1 Rep Power: 5	All that updateCoeffs() does, as defined in fvPatchField.C, is setting flag update_ to true: Code: template<class Type> void Foam::fvPatchField<Type>::updateCoeffs() { updated_ = true; }

May 28, 2022, 11:01		#18
Mars409 New Member Join Date: May 2020 Posts: 29 Blog Entries: 1 Rep Power: 5	The fixedFluxPressure boundary condition and the constrainPressure() function are now explained in a detailed openFOAM Wiki article on the SimpleFOAM solver: https://openfoamwiki.net/index.php/S...ssure_equation Mahmoud Abbaszadeh likes this.