[Sugajen]

Hi all,

After using OF for a while, I have a very basic question Pressure in OF is specified after dividing it by by rho. But, which Pressure do we specify in 0 folder?

1. Is it static pressure or total pressure ?
2. Is it gauge pressure or absolute pressure ?

Here is the context in which I am asking these. The case is incompressible, laminar solved using simpleFoam and is driven by velocity at the inlet. But it also has a high pressure, say 3x10^5 Pa absolute at the outlet. The inlet pressure BC is zeroGradient. What do we specify as BC for outlet ? Is it (3x10^5 - Atm pressure)/rho or just (3x10^5)/rho? I am sure that it is static but not entirely sure about gauge vs absolute.

After reading the following discussions and documentation, I only got more confused rather than clarity

http://www.openfoam.com/documentatio...-pressure.html
Which pressure OpenFOAM use for incompressible flow? P/rho or (P-101325)/rho ?
Reference pressure in OpenFOAM

Any comments or links to the OF documentation addressing this would be great

Thanks!

[piu58]

If you calculate incompresible the absolute value for pressure doesn't count It are the pressure differences which makes the fluid flow.
You may choose 0 as reference pressure (instead of yourrather high value). The solution should remain equal.

Absolute values play a role if you give two or more pressures. But even then only the differences count.

[Sugajen]

Thank you for your reply.

But do tell me this, when we specify 0 at outlet, what does it mean? Is it gauge pressure? If so, to get the actual pressure should we add it to atmospheric pressure. Else does it mean it is vacuum pressure ?

Thanks in advance!

[piu58]

It may be the pressure you are imagine there. It doesn't count if you add a Constant pressure everywhere.

Sent from my Gigaset GS160 using CFD Online Forum mobile app

[Santiago]

In incompressible flows pressure is a diagnostic variable, and has no physical meaning. It only has a mathematical meaning, as a lagrangian multiplier (more details in the book of Volker John, on FEM and navier stokes). The gradient of pressure does have physical meaning. This being said, the BC for pressure should be selected as to "minimize" mass conservation error.

Sent from my Lenovo A5000 using CFD Online Forum mobile app

[hooman.4028]

Originally Posted by Santiago

In incompressible flows pressure is a diagnostic variable, and has no physical meaning. It only has a mathematical meaning, as a lagrangian multiplier (more details in the book of Volker John, on FEM and navier stokes). The gradient of pressure does have physical meaning. This being said, the BC for pressure should be selected as to "minimize" mass conservation error.

Sent from my Lenovo A5000 using CFD Online Forum mobile app

That is true Santiago, but still some confusion here. Let's say you simply have a system which has to operate at a certain pressure, let's say A and you are asked to simulate the flow within this system from someone who has no idea about CFD. You are supposed to get back to the guy and tell him what pump to choose, how would you guide him?
In terms of working with OpenFoam, it is simply a fixed pressure at the outlet and this pressure does not have a physical meaning as you mentioned, but again this pressure can affect other equations which might be dependent on this outlet (operating) pressure. More specifically, how would you assume that your system is operating in atmospheric pressure? Would a 0 pressure at the outlet suffice? Thanks.

[Santiago]

Pressure obtained from PISO/SIMPLE are solved 'up to a constant'. Adding the atmospheric pressure to your field will give you an absolute pressure field. I never set a fixed pressure unless I have no other option than set zeroGradient on velocities. Note that zeroGradient is not a good condition for velocities, and should always be avoided. Lastly, it is the velocities that induce a certain pressure field not the contrary. More clearly, given a velocity field you can always calculate the pressure, but not the converse. So operating conditions for any system are determined given a satisfactory velocity field.

Sent from my Lenovo A5000 using CFD Online Forum mobile app

[BlnPhoenix]

Originally Posted by Santiago

Pressure obtained from PISO/SIMPLE are solved 'up to a constant'. Adding the atmospheric pressure to your field will give you an absolute pressure field. I never set a fixed pressure unless I have no other option than set zeroGradient on velocities. Note that zeroGradient is not a good condition for velocities, and should always be avoided. Lastly, it is the velocities that induce a certain pressure field not the contrary. More clearly, given a velocity field you can always calculate the pressure, but not the converse. So operating conditions for any system are determined given a satisfactory velocity field.

Hi, can you elaborate why it is not a good idea to set zeroGradient for velocity and fixedPressure = 0 at outlet? For me it has been common practice in OF to do so.

[Santiago]

zeroGradient does not correspond to the parabolic character of NS, in general reduces the solution to a L1 space. There has been extensive work on advection BC for NS. Look for Orlansky boundary condition. Physically, it does not preserve the structure of incoming eddies.

Sent from my Lenovo A5000 using CFD Online Forum mobile app

[hooman.4028]

Originally Posted by Santiago

zeroGradient does not correspond to the parabolic character of NS, in general reduces the solution to a L1 space. There has been extensive work on advection BC for NS. Look for Orlansky boundary condition. Physically, it does not preserve the structure of incoming eddies.

Sent from my Lenovo A5000 using CFD Online Forum mobile app

Thanks Santiago! Then I have three more questions, how about the pressure driven flows? I see that it is common to use total pressure at the inlet and fixed value at the outlet?

Also, from my understanding if adding atmospheric will give us the absolute pressure, it means that the pressure being solved is gauge. Correct? Then by adding the dynamic pressure from the velocity field we can find the total pressure?

The last question, what is the role of pRef here? I see it is always set as 0.

Thank you very much!

[Santiago]

1) if you set all pressure BC to zeroGradient or periodic, the inversion of the pressure poisson equation is ill-posed. Thus the need to set pRef. Nothing to do with a physical pressure.
2) pressure *does not* drive a flow, but when made a bodyforce by means of (miraculous) Gauss, i.e pressure gradient, it acts as a potential.
3) the term dP/dx_i in Momentum equation has different meanings depending on the system studied. For instance, when modelling gravity currents P is equal to the time-space pressure fluctuations plus the hydrostatic pressure plus the diagonal part of the stress tensor (in LES is important) plus a constant. So a much more basic answer has to be given: all bodyforces that can be written as the gradient of a potential make part of P.

Sent from my Lenovo A5000 using CFD Online Forum mobile app

[Tobi]

Hi all,

I just want to include a bit more of information here. First of all I agree with the statements given by Santiago especially for turbulent flows (back flow - how are the eddies coming back etc. - by the way does FOAM provide an Orlansky BC? - I don't make LES / DNS simulations and I am not so familiar).
In addition everything that is mentioned about the pressure is correct. If you derive the Navier-Stokes-Equation for incompressible fluids, you will find that the pressure p does not have any physical meaning. Only the gradient of p has a meaning. As it was already said, it is the driving force for your flow. Therefore, if you set a fixed value of pressure at the outlet to 0 or 1e5 does not influence your system because only the gradient is of physical meaning.

Case 1 p = 0 at outlet

• In that case you specify p at the outlet with an value of 0. Setting an inflow using U, you might see negative pressure values at the inlet or in the whole domain.

Case 2 p = 1e5 at outlet

• In that case you will not see negative pressure values but actually if you would make the gradient of p_outlet - p_Inlet, it would be the same values as in Case 1

Case 3 pressure driven flows

• The reason to specify totalPressure with (pressureInletVelocity) and fixedValue at the inlet and outlet is obvious.
• If one would specify fixedValue at the inlet and outlet, you will have a pressure gradient which will never vanish. If you go on in time, the gradient will accelerate your flow till infty.
• The totalPressure reduces the pressure at each face based on the flux that is coming in. E.g. the pressure at the inlet face is equal to the pressure you set minus the kinematic pressure.
• You can see that the increase of velocity will decrease the values of the pressure at the inlet and thus the total pressure gradient and therefore the acceleration of the flud.
• At the end you will have an established flow that is in equilibrium.
• By the way you simply can make that test with a normal pipe flow.

Pressure values

As already mentioned you can set p to any value because only the gradients matter here (still talking about incompressible cases). Therefore, if you would like to know the absolute pressure value, you can do it as follow:

• You know that the pressure at the outlet is 1.5e5 Pa (atmospheric + 0.5 bar)
• Incompressible means divide by density
• Then set this values of 1.5e5 Pa / density at the outlet
• After the calculation you have to multiply the pressure by the density again (to get the values in Pascal)
• Then you would have the absolute pressure values

I hope I did not make any mistake here but it should be fine. As you can see, the dividing and multiplying step could be removed but this is the logical way. Again, as Santiago already stated, the pressure here has no physical meaning. The solver would also run if you set p at the outlet to a value of -141235.

By the way Philippo was talking about that here too: Outflow boundary condition for LES/DNS

[Santiago]

Originally Posted by Tobi

Hi all,

I just want to include a bit more of information here. First of all I agree with the statements given by Santiago especially for turbulent flows (back flow - how are the eddies coming back etc. - by the way does FOAM provide an Orlansky BC? - I don't make LES / DNS simulations and I am not so familiar).
In addition everything that is mentioned about the pressure is correct. If you derive the Navier-Stokes-Equation for incompressible fluids, you will find that the pressure p does not have any physical meaning. Only the gradient of p has a meaning. As it was already said, it is the driving force for your flow. Therefore, if you set a fixed value of pressure at the outlet to 0 or 1e5 does not influence your system because only the gradient is of physical meaning.

Case 1 p = 0 at outlet

• In that case you specify p at the outlet with an value of 0. Setting an inflow using U, you might see negative pressure values at the inlet or in the whole domain.

Case 2 p = 1e5 at outlet

• In that case you will not see negative pressure values but actually if you would make the gradient of p_outlet - p_cellI it would be the same values as in Case 1

Case 3 pressure driven flows

• The reason to specify totalPressure with (pressureInletVelocity) and fixedValue at the outlet is obvious.
• If one would specify fixedValue at the inlet and outlet, you will have a pressure gradient which will never vanish. If you go on in time, the gradient will accelerate your flow till infty.
• The totalPressure reduces the pressure at each face based on the flux that is coming in. E.g. the pressure at the inlet face is equal to the pressure you set minus the kinematic pressure.
• You can see that the increase of velocity will decrease the values of the pressure at the inlet and thus the total pressure gradient and therefore the acceleration of the flud.
• At the end you will have an established flow that is in equilibrium.
• By the way you simply can make that test with a normal pipe flow.

Pressure values

As already mentioned you can set p to any value because only the gradients matters here (still talking about incompressible cases). Therefore if you would like to know the absolute pressure value, you can do it as follow:

• You know that the pressure at the outlet is 1.5e5 Pa (atmospheric + 0.5 bar)
• Incompressible means divide by density
• Then set this values as outlet
• After the calculation you have to multiply the pressure by the density again (to get the values in Pascal again)
• Then you would have the absolute pressure values

I hope I did not make any mistake here but it should be fine. As you can see, the dividing and multiplying step could be removed but this is the logical way. Again, as Santiago already stated, the pressure here has no physical meaning. The solver would also run if you set p at the outlet to a value of -141235.

By the way Philippo was talking about that here too: Outflow boundary condition for LES/DNS

The Orlansky BC is not "implemented" for PISO. nevertheless, in foam-extend there is a BC called 'advective' which is used for blast simulations, and can serve as a template for the Orlansky.

Sent from my Lenovo A5000 using CFD Online Forum mobile app

[Tobi]

Thanks for the hint.
Never came across about that boundary condition. Thank you again. By the way this BC is also available in the other derivatives, Foundation and ESI.

[allett02015]

I can confirm that in the openfoam version 16.12 and newer the advective (or in some cases also called convective) boundary conditions is implemented

[svramana]

hello sir,
This is about incompressible fluid. can you please explain what about compressible fluid. because I'm working on gas turbine and so working fluid is compressible. I didn't saw anyone talking about compressible fluid.

[Tobi]

Originally Posted by allett02015

I can confirm that in the openfoam version 16.12 and newer the advective (or in some cases also called convective) boundary conditions is implemented

The definition is as follow:

If one is talking about the momentum then we talk about convection (Velocity field).
If one is talking about anything thing else which is transported by the velocity field, then we say that the field is advected.


Generally, people always say convected.

hello sir,
This is about incompressible fluid. can you please explain what about compressible fluid. because I'm working on gas turbine and so working fluid is compressible. I didn't saw anyone talking about compressible fluid.

What are you referring to? Are you talking about pressure in compressible fluids?

[svramana]

hello sir,

Originally Posted by Tobi

What are you referring to? Are you talking about pressure in compressible fluids?

Yes, I'm talking about pressure in compressible fluids. In above post you have explained very well about BCs of pressure in incompressible fluid. I want to know about compressible fluid.

[waradevivek]

Did anyone got the pressure considerations for compressible flows. I have also got stuck into similar problem.

[miotto]

Originally Posted by Tobi

Hi all,

I just want to include a bit more of information here. First of all I agree with the statements given by Santiago especially for turbulent flows (back flow - how are the eddies coming back etc. - by the way does FOAM provide an Orlansky BC? - I don't make LES / DNS simulations and I am not so familiar).
In addition everything that is mentioned about the pressure is correct. If you derive the Navier-Stokes-Equation for incompressible fluids, you will find that the pressure p does not have any physical meaning. Only the gradient of p has a meaning. As it was already said, it is the driving force for your flow. Therefore, if you set a fixed value of pressure at the outlet to 0 or 1e5 does not influence your system because only the gradient is of physical meaning.

Case 1 p = 0 at outlet

• In that case you specify p at the outlet with an value of 0. Setting an inflow using U, you might see negative pressure values at the inlet or in the whole domain.

Case 2 p = 1e5 at outlet

• In that case you will not see negative pressure values but actually if you would make the gradient of p_outlet - p_Inlet, it would be the same values as in Case 1

Case 3 pressure driven flows

• The reason to specify totalPressure with (pressureInletVelocity) and fixedValue at the inlet and outlet is obvious.
• If one would specify fixedValue at the inlet and outlet, you will have a pressure gradient which will never vanish. If you go on in time, the gradient will accelerate your flow till infty.
• The totalPressure reduces the pressure at each face based on the flux that is coming in. E.g. the pressure at the inlet face is equal to the pressure you set minus the kinematic pressure.
• You can see that the increase of velocity will decrease the values of the pressure at the inlet and thus the total pressure gradient and therefore the acceleration of the flud.
• At the end you will have an established flow that is in equilibrium.
• By the way you simply can make that test with a normal pipe flow.

Pressure values

As already mentioned you can set p to any value because only the gradients matter here (still talking about incompressible cases). Therefore, if you would like to know the absolute pressure value, you can do it as follow:

• You know that the pressure at the outlet is 1.5e5 Pa (atmospheric + 0.5 bar)
• Incompressible means divide by density
• Then set this values of 1.5e5 Pa / density at the outlet
• After the calculation you have to multiply the pressure by the density again (to get the values in Pascal)
• Then you would have the absolute pressure values

I hope I did not make any mistake here but it should be fine. As you can see, the dividing and multiplying step could be removed but this is the logical way. Again, as Santiago already stated, the pressure here has no physical meaning. The solver would also run if you set p at the outlet to a value of -141235.

By the way Philippo was talking about that here too: Outflow boundary condition for LES/DNS

Hi Tobi, thanks for the comprehensive answer.

You mentioned that

Incompressible means divide by density

But does it always? What about incompressible multi-phase solvers like InterFoam?
I think in this case one should simply use the pressure in Pa, correct?