
[Sponsors] 
Which pressure OpenFOAM use for incompressible flow? P/rho or (P101325)/rho ? 

LinkBack  Thread Tools  Search this Thread  Display Modes 
December 15, 2009, 04:59 
Which pressure OpenFOAM use for incompressible flow? P/rho or (P101325)/rho ?

#1 
Senior Member
Jiang
Join Date: Oct 2009
Location: Japan
Posts: 186
Rep Power: 16 
Dear Foamers:
I am a little confused about pressure for imcompressible flow. I want to know which pressure OpenFOAM uses. Because in outflow boundary, pressure value is fixed. So if you give zero, the pressure result will be very small. If you give 101325/rho, the pressure result will be large. in all the tutorials of OpenFOAM , in case/0 ,pressure is set to zero. If that means , the pressure set in P file is (Real Pressure  101325)/rho ? Thank you very much! 

December 15, 2009, 15:23 

#2 
New Member
Join Date: Mar 2009
Posts: 27
Rep Power: 17 
Isn't the pressure already divided by rho?
So the real pressure would be p*rho and then if you have 0 at outlet add atmospheric pressure so: p*rho + 101325 But you should see my post about pressure and knowbody has answered yet. http://www.cfdonline.com/Forums/ope...cellsize.html I suspect pressure is not being calculated correctly because it varies too much with cell size. If so you can't use the pressure value. 

October 11, 2013, 11:37 

#3  
Member
Join Date: Aug 2013
Posts: 50
Rep Power: 12 
Quote:
thanks 

October 11, 2013, 22:00 

#4 
Senior Member
Fumiya Nozaki
Join Date: Jun 2010
Location: Yokohama, Japan
Posts: 266
Blog Entries: 1
Rep Power: 18 
You can get the real pressure value (that is not divided by rho) using the formula
that jugghead wrote and you can find the rho value by consulting the physical property books at your simulation condition. Hope this helps, Fumiya 

October 12, 2013, 03:53 

#5  
Member
Join Date: Aug 2013
Posts: 50
Rep Power: 12 
Quote:
nu=mu/rho So how can i just get the value from the book. Isnt the simplefoam or other incompressible solver default value used? So what is the default value then? i have done the solver, with nu 1.5exp5 (from motorbike tutorial) Now i need the rho value based on that nu or based on the motorbike tutorial. Thanks 

October 12, 2013, 05:22 

#6 
Senior Member
Fumiya Nozaki
Join Date: Jun 2010
Location: Yokohama, Japan
Posts: 266
Blog Entries: 1
Rep Power: 18 
Hi nash,
If you look at the table(http://www.engineeringtoolbox.com/ai...iesd_156.html), you can find that the kinematic viscosity(nu) value is nearly equal to 1.5e5 at 20 degrees Celsius and the density(rho) value is 1.205 kg/m^3 at this temperature. So, the motor bike tutorial solves the flow on these conditions if the working fluid is air. If you try to do another simulation at different condition(different temperature or fluid etc.), you can find the nu and rho value from books and set nu value in the transportProperties dictionary. When your simulation finishes, you can get the real pressure value using the formula that jugghead wrote and the density value you will have found. 

October 12, 2013, 05:46 

#7  
Member
Join Date: Aug 2013
Posts: 50
Rep Power: 12 
Quote:
Now i would like to ask, if i want to get the exact pressure direct from the simulation, i plan to set the rho to 1. So i need to set nu. But i dont know the mu. Any idea? Temperature is at 20 degree celcius. Isnt okay if i do so? Thanks again for your help 

October 29, 2014, 06:56 

#9 
Member
Join Date: Aug 2011
Posts: 89
Rep Power: 14 
Hello together,
I know this thread is older but I am a little confused at the moment concerning the pressure. If I use the incompressible solver interFoam and set the pressure to 0 in 0/p, I sometimes get a negative pressure p. Is it also true in this case that I calculate the "real" static pressure with p + 101325? Thanks a lot for your help idefix 

November 21, 2014, 01:26 

#10 
Member
Artem Shaklein
Join Date: Feb 2010
Location: Russia, Izhevsk
Posts: 43
Rep Power: 16 
Hello, idefix.
In incompressible limit , so only affects a solution. It doesn't matter whether absolute static pressure p_abs[0] = 1e5 or p_abs[0] = 2e5 (by the way, p_abs[0] = 0 can be used as well, but it is nonsense, because in vacuum just small amount of matter is presented and it can't be modeled by continuum mechanics theory). If density is constant, it's useful to divide all equations by density, so to recover abs pressure one has to do the math . In this case pressure (0/p) has dimensions [Pa/(kg/m^3)]. But this approach can be used in general case as well (just consider a number of digits to store: 1.013250001e5 vs 1.0e4). To recover pressure one needs next . In this case pressure (0/p) has dimensions [Pa]. I looked inside interFoam case and found that 0/p has [Pa] dimensions. So you should go with . 

February 5, 2015, 10:53 

#11 
Senior Member

Just a question for confirmation, as I'm getting confuse with my results, in order to see how to change my BC.
In 0/U I defined pressureInletvelocity and in 0/p I defined total pressure for inlet and set it equal to 0, so I defined: total = static + dynamic > 0 = 0 + rho*U^2/2 (value for U= (0 0 0) > all is zero) When I plot a slice on paraview, what pressure I get? static pressure divided by rho? total pressure divided by rho? or in other way to ask, is pressure calculated by openfoam the static one or the total pressure? thanks a lot. Bye 

January 5, 2016, 11:17 

#12  
Member
Join Date: Dec 2014
Posts: 50
Rep Power: 11 
Quote:
Thanks! 

April 22, 2016, 04:38 

#13  
New Member

Quote:
Notations  p = static pressure ptot = total pressure rho = density to my knowledge, for incompressible flows, OF solves for p/rho. You can find total pressure (ptot = p + 1/2 * rho *U^2) using the ptot utility. 

August 10, 2018, 12:55 

#14 
New Member
Chayanit Nigaltia
Join Date: Jan 2018
Posts: 29
Rep Power: 8 
If I define my own rho and rhoInf, the will the static pressure be normalised by my value of rho?
Please help. 

August 13, 2018, 05:22 
it is simple

#15 
Member
ijaz fazil
Join Date: Apr 2013
Location: Singapore
Posts: 73
Rep Power: 13 
You have to provide boundary value
pressure(density*g*height) For example if you want to specify pressure to be zero then enter the value 0(density*g*height) Make sure that your g value specified correctly in constant folder. 

August 14, 2018, 04:40 

#16 
New Member
Chayanit Nigaltia
Join Date: Jan 2018
Posts: 29
Rep Power: 8 
Thanks Ijaz
Since the pressure value is already normalised by density in openfoam( I think they have used a value of 1.2) So now do I have to change the source code and then compile.Or by simply stating my free stream density and acceleration due to gravity, I will have my calculations correct. 

August 14, 2018, 04:57 
for interfoam pressure is not normalised

#17 
Member
ijaz fazil
Join Date: Apr 2013
Location: Singapore
Posts: 73
Rep Power: 13 
Hi
But for interFoam alone pressure should not be normalised with density, might be because you have two different fluids with different density, so we have to use the actual value of pressure. For example if atmospheric pressure is zero, then use that value to define the boundary. 

Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Pressure Drop  Please Help  Simple Pipe Flow  Joe A.  FLUENT  2  April 23, 2007 07:50 
FLOW AROUND A PLATE_NEGATIVE ABSOLUTE PRESSURE????  tania  FLUENT  11  March 23, 2004 08:51 
what the result is negatif pressure at inlet  chong chee nan  FLUENT  0  December 29, 2001 05:13 
mass flow inlet  Denis Tschumperle  FLUENT  7  August 9, 2000 02:19 
Hydrostatic pressure in 2phase flow modeling (CFX4.2)  HB &DS  CFX  0  January 9, 2000 13:19 