
[Sponsors] 
In what unit is pressure measured on OpenFOAM? 

LinkBack  Thread Tools  Search this Thread  Display Modes 
January 26, 2021, 14:19 
In what unit is pressure measured on OpenFOAM?

#1 
New Member
Matheus
Join Date: Jan 2020
Posts: 9
Rep Power: 4 
Hi guys, while checking the results of my simulations I noticed that the pressure has an unfamiliar value, the speed vector seems to have the expected value but the same doesn't apply to the pressure. I'm simulating a pressure drop through an orifice plate inside a pipe and comparing the values with a previous experiment, the pressure at the gages were measured at 1.5 PSI (10.3Kpa) before the orifice plate and 0 PSI after. The calculated pressures for the same experiment were 1.564 PSI and 0.264 PSI respectively, which are close to the experimental result, but when I run the simulation the value for pressure before the plate is 0.764 and 0.267, after researching a little I read that openFOAM uses the pressure normalized by rho (p/rho), so, in order to find the value of the pressure I need to multiply the value that I found and rho? Even after multiplying the value in pascals is too low to be accurate (around 764pa and 267pa)
I set the boundary conditions following the pitzdaily tutorial, maybe I missed something at the inlet boundary condition, I set all the boundaries to be zerogradient for the pressure, except the outlet which is set as fixedvalue: uniform 0. I would be very thankful if any of you guys could help me out. 

January 26, 2021, 15:14 

#2 
Senior Member
Mark Olesen
Join Date: Mar 2009
Location: https://olesenm.github.io/
Posts: 1,503
Rep Power: 35 
Pressure is in Pascals for compressible flow solvers, and the"p/rho" for incompressible


January 29, 2021, 18:12 

#3 
Member
Ran
Join Date: Aug 2016
Posts: 69
Rep Power: 8 
I am just curious that "p/rho" is used in OF.
It seems to have some calculation advantages but I do not know the details
__________________
Yours in CFD, Ran 

January 30, 2021, 17:18 

#4  
Senior Member
Mark Olesen
Join Date: Mar 2009
Location: https://olesenm.github.io/
Posts: 1,503
Rep Power: 35 
Quote:
Well if the simulation is incompressible you can either have an implied constant density to drag through all the equations (eg, multiplying by one in various places) or simply do away with density in the equations by more or less factoring it into pressure (p = p/rho, and rho == 1) thus giving the units in question. 

February 1, 2021, 08:41 

#5 
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Tussenhausen
Posts: 2,677
Blog Entries: 6
Rep Power: 49 
I refer to my book "Mathematics, Numerics, Derivations and OpenFOAM". Here, all equations are described.
As Mark already said, if we have incompressible solvers it is ment that the density is constant and not changing, e.g., by compression or expansion or thermal behavior. As the density is constant, we can take the density out of all derivatives and can cancel via rho. Thus, in all terms including rho, it vanishes and the terms that do not have the density included (such as the pressure term) are divided by the density. Hence, p/rho = p* for incompressible flows. Nevertheless, for incompressible flows the pressure does not have the physical meaning as a "real" pressure as only the pressure gradients are of importantance. Thus, one can see negative pressure values p*.
__________________
Keep foaming, Tobias Holzmann 

February 1, 2021, 13:15 

#6 
Member
Ran
Join Date: Aug 2016
Posts: 69
Rep Power: 8 
I know that, for the incomprensible case, the pressure is usually not
in [Pa] but it is divided by the fluid density (so the unit is m^2/s^2) in OpenFOAM. In order to get the pressure in the unit [Pa], one needs to multiply the result from OpenFOAM by the density. However, this extra step makes me think there might be advantages in using such a simplification in incompressible solver. Imaging a new user would expect to set the pressure in the simulation and expect the calculation result is immediately available to compare to their experiment tests. In addition, introducing the density into the incompressible solver might simplify the codebase. I don't know the OOP details, but just a guess. "the pressure does not have the physical meaning as a "real" pressure as only the pressure gradients are of importance." This perspective is interesting. Is there any other fundamental measurement that exists that only has importance to their gradient but not themselves? For example, the second, metre, kilogram, ampere, kelvin, mole, candela.
__________________
Yours in CFD, Ran 

February 2, 2021, 14:55 

#7 
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Tussenhausen
Posts: 2,677
Blog Entries: 6
Rep Power: 49 
Sure there is a benefit. If you use a density field in the equations, we have to interpolate these quantities to the faces even though it is everywhere the same because we calculate the face fluxes using U and rho in the cell center. Hence, we have to interpolate it to the faces. If we remove the density (as it is a constant) we only need to interpolate U and not both U and rho.
__________________
Keep foaming, Tobias Holzmann 

Tags 
openfoam, orifice plate, pressure 
Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Map of the OpenFOAM Forum  Understanding where to post your questions!  wyldckat  OpenFOAM  10  September 2, 2021 06:29 
What is difference between static pressure and gauge pressure?  aja1345  FLUENT  1  July 20, 2018 21:05 
OpenFOAM Training JanJul 2017, Virtual, London, Houston, Berlin  CFDFoundation  OpenFOAM Announcements from Other Sources  0  January 4, 2017 07:15 
Suggestion for a new subforum at OpenFOAM's Forum  wyldckat  Site Help, Feedback & Discussions  20  October 28, 2014 10:04 
measured pressure in the discharge pipe jumps  Jan  Main CFD Forum  1  October 30, 2006 08:54 