
[Sponsors] 
July 6, 2017, 21:23 
Pressure in OpenFOAM

#1 
Member
Sugajen
Join Date: Jan 2012
Location: Tempe, USA
Posts: 52
Rep Power: 9 
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 (P101325)/rho ? Reference pressure in OpenFOAM Any comments or links to the OF documentation addressing this would be great Thanks! 

July 7, 2017, 00:42 

#2 
Senior Member
Uwe Pilz
Join Date: Feb 2017
Location: Leipzig, Germany
Posts: 590
Rep Power: 7 
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.
__________________
Uwe Pilz  Die der Hauptbewegung überlagerte Schwankungsbewegung ist in ihren Einzelheiten so hoffnungslos kompliziert, daß ihre theoretische Berechnung aussichtslos erscheint. (Hermann Schlichting, 1950) 

July 7, 2017, 16:10 

#3 
Member
Sugajen
Join Date: Jan 2012
Location: Tempe, USA
Posts: 52
Rep Power: 9 
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! 

July 8, 2017, 00:44 

#4 
Senior Member
Uwe Pilz
Join Date: Feb 2017
Location: Leipzig, Germany
Posts: 590
Rep Power: 7 
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
__________________
Uwe Pilz  Die der Hauptbewegung überlagerte Schwankungsbewegung ist in ihren Einzelheiten so hoffnungslos kompliziert, daß ihre theoretische Berechnung aussichtslos erscheint. (Hermann Schlichting, 1950) 

July 8, 2017, 08:10 

#5 
Senior Member
Santiago Lopez Castano
Join Date: Nov 2012
Posts: 198
Rep Power: 8 
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 

July 10, 2017, 20:53 

#6  
Member
Hooman
Join Date: Apr 2011
Posts: 35
Rep Power: 10 
Quote:
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. 

July 11, 2017, 04:31 

#7 
Senior Member
Santiago Lopez Castano
Join Date: Nov 2012
Posts: 198
Rep Power: 8 
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 

July 11, 2017, 05:00 

#8  
Senior Member
Join Date: Aug 2014
Location: Germany
Posts: 246
Rep Power: 7 
Quote:


July 11, 2017, 05:32 

#9 
Senior Member
Santiago Lopez Castano
Join Date: Nov 2012
Posts: 198
Rep Power: 8 
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 

July 11, 2017, 10:15 

#10  
Member
Hooman
Join Date: Apr 2011
Posts: 35
Rep Power: 10 
Quote:
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! 

July 11, 2017, 11:50 

#11 
Senior Member
Santiago Lopez Castano
Join Date: Nov 2012
Posts: 198
Rep Power: 8 
1) if you set all pressure BC to zeroGradient or periodic, the inversion of the pressure poisson equation is illposed. 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 timespace 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 

July 17, 2017, 08:17 

#12 
Super Moderator

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 NavierStokesEquation 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
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:
By the way Philippo was talking about that here too: Outflow boundary condition for LES/DNS
__________________
Keep foaming, Tobias Holzmann 

July 17, 2017, 10:15 

#13  
Senior Member
Santiago Lopez Castano
Join Date: Nov 2012
Posts: 198
Rep Power: 8 
Quote:
Sent from my Lenovo A5000 using CFD Online Forum mobile app 

July 17, 2017, 10:20 

#14 
Super Moderator

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.
__________________
Keep foaming, Tobias Holzmann 

May 24, 2018, 01:44 

#15 
New Member
Michael
Join Date: Feb 2015
Posts: 18
Rep Power: 6 
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


June 20, 2018, 05:08 

#16 
Member
Ramana
Join Date: Jul 2017
Location: India
Posts: 58
Rep Power: 3 
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. 

June 20, 2018, 12:12 

#17  
Super Moderator

Quote:
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. Quote:
__________________
Keep foaming, Tobias Holzmann 

June 27, 2018, 06:21 

#18 
Member
Ramana
Join Date: Jul 2017
Location: India
Posts: 58
Rep Power: 3 
hello sir,
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. 

July 31, 2018, 08:06 

#19 
New Member
vivek
Join Date: Oct 2011
Location: Pune Maharashtra
Posts: 6
Rep Power: 9 
Did anyone got the pressure considerations for compressible flows. I have also got stuck into similar problem.


Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
question regarding LES of pipe flow  pimpleFoam  Dan1788  OpenFOAM Running, Solving & CFD  37  December 26, 2017 14:42 
Map of the OpenFOAM Forum  Understanding where to post your questions!  wyldckat  OpenFOAM  9  March 30, 2017 05:19 
interFoam (HELYXOS) pressure boundary conditions  SFr  OpenFOAM Running, Solving & CFD  8  June 23, 2016 16:36 
CFX Solver stopped with error when requested for backup during solver running  Mfaizan  CFX  40  May 13, 2016 06:50 
OpenFOAM Training, London, Chicago, Munich, SepOct 2015  cfd.direct  OpenFOAM Announcements from Other Sources  2  August 31, 2015 13:36 