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

In what unit is pressure measured on OpenFOAM?

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

Like Tree2Likes
  • 1 Post By olesen
  • 1 Post By olesen

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   January 26, 2021, 14:19
Default In what unit is pressure measured on OpenFOAM?
  #1
New Member
 
Matheus
Join Date: Jan 2020
Posts: 9
Rep Power: 4
Matheus.Costa is on a distinguished road
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.
Matheus.Costa is offline   Reply With Quote

Old   January 26, 2021, 15:14
Default
  #2
Senior Member
 
Mark Olesen
Join Date: Mar 2009
Location: https://olesenm.github.io/
Posts: 1,503
Rep Power: 35
olesen will become famous soon enougholesen will become famous soon enough
Pressure is in Pascals for compressible flow solvers, and the"p/rho" for incompressible
Matheus.Costa likes this.
olesen is offline   Reply With Quote

Old   January 29, 2021, 18:12
Default
  #3
Member
 
Ran
Join Date: Aug 2016
Posts: 69
Rep Power: 8
random_ran is on a distinguished road
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
random_ran is offline   Reply With Quote

Old   January 30, 2021, 17:18
Default
  #4
Senior Member
 
Mark Olesen
Join Date: Mar 2009
Location: https://olesenm.github.io/
Posts: 1,503
Rep Power: 35
olesen will become famous soon enougholesen will become famous soon enough
Quote:
Originally Posted by random_ran View Post
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

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.
Tobi likes this.
olesen is offline   Reply With Quote

Old   February 1, 2021, 08:41
Default
  #5
Super Moderator
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Tussenhausen
Posts: 2,677
Blog Entries: 6
Rep Power: 49
Tobi has a spectacular aura aboutTobi has a spectacular aura aboutTobi has a spectacular aura about
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
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
Tobi is offline   Reply With Quote

Old   February 1, 2021, 13:15
Default
  #6
Member
 
Ran
Join Date: Aug 2016
Posts: 69
Rep Power: 8
random_ran is on a distinguished road
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
random_ran is offline   Reply With Quote

Old   February 2, 2021, 14:55
Default
  #7
Super Moderator
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Tussenhausen
Posts: 2,677
Blog Entries: 6
Rep Power: 49
Tobi has a spectacular aura aboutTobi has a spectacular aura aboutTobi has a spectacular aura about
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
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
Tobi is offline   Reply With Quote

Reply

Tags
openfoam, orifice plate, pressure

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


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 Jan-Jul 2017, Virtual, London, Houston, Berlin CFDFoundation OpenFOAM Announcements from Other Sources 0 January 4, 2017 07:15
Suggestion for a new sub-forum 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


All times are GMT -4. The time now is 17:08.