CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM

Which pressure OpenFOAM use for incompressible flow? P/rho or (P-101325)/rho ?

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree3Likes
  • 1 Post By panda60
  • 1 Post By jugghead
  • 1 Post By fumiya

Reply
 
LinkBack Thread Tools Display Modes
Old   December 15, 2009, 05:59
Default Which pressure OpenFOAM use for incompressible flow? P/rho or (P-101325)/rho ?
  #1
Senior Member
 
Jiang
Join Date: Oct 2009
Location: Japan
Posts: 186
Rep Power: 7
panda60 is on a distinguished road
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!
rv82 likes this.
panda60 is offline   Reply With Quote

Old   December 15, 2009, 16:23
Default
  #2
New Member
 
Join Date: Mar 2009
Posts: 27
Rep Power: 8
jugghead is on a distinguished road
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.cfd-online.com/Forums/ope...cell-size.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.
vbnhfylbh likes this.
jugghead is offline   Reply With Quote

Old   October 11, 2013, 11:37
Default
  #3
Member
 
Join Date: Aug 2013
Posts: 50
Rep Power: 3
nash is on a distinguished road
Quote:
Originally Posted by jugghead View Post
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.cfd-online.com/Forums/ope...cell-size.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.
may i know which default value of rho is used by simpleFoam (incompressible solver)? Because i need to have the right value for my pressure since i need to do performance curve of my fan simulation.

thanks
nash is offline   Reply With Quote

Old   October 11, 2013, 22:00
Default
  #4
Senior Member
 
Fumiya Nozaki
Join Date: Jun 2010
Location: Yokohama, Japan
Posts: 168
Rep Power: 7
fumiya is on a distinguished road
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
fumiya is offline   Reply With Quote

Old   October 12, 2013, 03:53
Default
  #5
Member
 
Join Date: Aug 2013
Posts: 50
Rep Power: 3
nash is on a distinguished road
Quote:
Originally Posted by fumiya View Post
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
basically one defines the nu value in transport properties. The nu value is given by this equation

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 1.5exp-5 (from motorbike tutorial)
Now i need the rho value based on that nu or based on the motorbike tutorial.
Thanks
nash is offline   Reply With Quote

Old   October 12, 2013, 05:22
Default
  #6
Senior Member
 
Fumiya Nozaki
Join Date: Jun 2010
Location: Yokohama, Japan
Posts: 168
Rep Power: 7
fumiya is on a distinguished road
Hi nash,

If you look at the table(http://www.engineeringtoolbox.com/ai...ies-d_156.html),
you can find that the kinematic viscosity(nu) value is nearly equal to 1.5e-5 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.
nash likes this.
fumiya is offline   Reply With Quote

Old   October 12, 2013, 05:46
Default
  #7
Member
 
Join Date: Aug 2013
Posts: 50
Rep Power: 3
nash is on a distinguished road
Quote:
Originally Posted by fumiya View Post
Hi nash,

If you look at the table(http://www.engineeringtoolbox.com/ai...ies-d_156.html),
you can find that the kinematic viscosity(nu) value is nearly equal to 1.5e-5 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.
Thanks for the explanation.

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
nash is offline   Reply With Quote

Old   October 12, 2013, 10:26
Default
  #8
Senior Member
 
Fumiya Nozaki
Join Date: Jun 2010
Location: Yokohama, Japan
Posts: 168
Rep Power: 7
fumiya is on a distinguished road
I think it's not possible and it is easier to multiply the result by rho after calculation.

Fumiya
fumiya is offline   Reply With Quote

Old   October 29, 2014, 07:56
Default
  #9
Member
 
Join Date: Aug 2011
Posts: 74
Rep Power: 5
idefix is on a distinguished road
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
idefix is offline   Reply With Quote

Old   November 21, 2014, 02:26
Default
  #10
Member
 
Artem Shaklein
Join Date: Feb 2010
Location: Russia, Izhevsk
Posts: 43
Rep Power: 7
ARTem is on a distinguished road
Hello, idefix.
In incompressible limit \rho \ne f (p), so only \mathrm{grad} p 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 p_{stat}^{abs} = p_{stat}^{relative} \rho + p_{stat}^{reference}. 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 1.0e-4). To recover pressure one needs next p_{stat}^{abs} = p_{stat}^{relative} + p_{stat}^{reference}. 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 p_{stat}^{abs} = p_{stat}^{relative} + p_{stat}^{reference}.
ARTem is offline   Reply With Quote

Old   February 5, 2015, 11:53
Default
  #11
Senior Member
 
M. C.
Join Date: May 2013
Location: Italy
Posts: 100
Rep Power: 4
student666 is on a distinguished road
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
student666 is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


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 09:51
what the result is negatif pressure at inlet chong chee nan FLUENT 0 December 29, 2001 06:13
mass flow inlet Denis Tschumperle FLUENT 7 August 9, 2000 02:19
Hydrostatic pressure in 2-phase flow modeling (CFX4.2) HB &DS CFX 0 January 9, 2000 14:19


All times are GMT -4. The time now is 03:29.