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

Reference pressure in OpenFOAM

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

Like Tree14Likes
  • 6 Post By alberto
  • 7 Post By alberto
  • 1 Post By Fine

Reply
 
LinkBack Thread Tools Display Modes
Old   May 13, 2010, 08:17
Default Reference pressure in OpenFOAM
  #1
New Member
 
satish
Join Date: Apr 2010
Posts: 6
Rep Power: 7
P.Satish is on a distinguished road
Hi!

I am new to openfoam and I have a very small query.

In cfd solvers, there is an option for Operation pressures, where I can enter 1 atm so at the boundaries I can enter the guage pressure as the operating pressure is 1atm.

Where is the option of operating pressure in OpenFOAM.

In unsteady solver in fvSolution folder, there its clearly mentioned for solvers
p{
}
U{
}
PISO
{
nCorrectors 2;
nNonOrthogonal Correctors 0;
pRefCell 0;
pRefValue 0;
}

so in the pressure velocity coupling PISO, there pressure reference value is showing 0, so what ever the pressure boundary value I enter at inlet and outlet makes the pressure absolute one. Please correct me whether the above pRefValue is same as the operating pressure in Fluent or not.

When it comes to steady state case

when I had gone to the similar folder

it shows

SIMPLE
{ nNonOrthogaonalCorrectors 0;
}

there is no pref value entered there?

do I have to type the same there, like what is there in PISO in unsteady solver?

or by default Reference pressure is zero internally and what ever the value of pressure I enter at inlet/outlet boundaries becomes absolute pressure in steady state cases?

Please help me in clarifying my query.
P.Satish is offline   Reply With Quote

Old   May 14, 2010, 01:17
Default
  #2
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,904
Rep Power: 26
alberto will become famous soon enoughalberto will become famous soon enough
Hi,

in OpenFOAM pRef is used only if your boundary conditions are set in such a way not to prescribe any reference for the pressure.

So, for example, if you open a duct open to the athmosphere at the outlet, and you have the velocity specified at the inlet, you should specify p equal to zero at the outlet (in incompressible flows, if you specify 1 it doesn't make any difference, you simply translate the values of the pressure in your whole domain of the same difference).

If you have a simulation where p has only Neumann (zeroGradient) conditions, the pRef value will be used, setting p = pRefVal in the cell of index pRefCell.

The values of pRefCell and pRefValue are always specified in the PISO/SIMPLE/PIMPLE subdictionary in fvSolution.

Best,
me.ouda, Alhasan, mgg and 3 others like this.
__________________
Alberto Passalacqua

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats.
OpenQBMM - An open-source implementation of quadrature-based moment methods.

To obtain more accurate answers, please specify the version of OpenFOAM you are using.
alberto is offline   Reply With Quote

Old   May 14, 2010, 05:27
Default
  #3
New Member
 
satish
Join Date: Apr 2010
Posts: 6
Rep Power: 7
P.Satish is on a distinguished road
Alberto Thanks for ur reply.

You are saying the pref will be used only when we give the condition pgradient = 0 at the inlet/outlet. and it wont use if we directly specify the outlet/inlet pressure as 0? Please correct me if I am wrong.

In fluent, if we specify pref=1atm, then if we entering a guage perssure of
0 atm at outlet then we can directly enter the value 0.

even if I am giving the perssure boundary condition p=0 at outlet, there wont be any wrong in specifying the pref value = 0 in tne fvSolution file, right?

when I am using a steady state case, do I have to clearly enter "nCorrectors" as 1, or by default it takes as one inside?

what is the value given for "nNonOrthogonal Correctors" for a tetra mesh?
P.Satish is offline   Reply With Quote

Old   May 14, 2010, 12:13
Default
  #4
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,904
Rep Power: 26
alberto will become famous soon enoughalberto will become famous soon enough
Quote:
Originally Posted by P.Satish View Post
Alberto Thanks for ur reply.

You are saying the pref will be used only when we give the condition pgradient = 0 at the inlet/outlet. and it wont use if we directly specify the outlet/inlet pressure as 0? Please correct me if I am wrong.
This actually depends on the solver. In some solver (i.e. pisoFoam) the reference is set using directly

Code:
Eqn.setReference(pRefCell, pRefValue);
In others the reference is set only if required.

Quote:
In fluent, if we specify pref=1atm, then if we entering a guage perssure of
0 atm at outlet then we can directly enter the value 0.

even if I am giving the perssure boundary condition p=0 at outlet, there wont be any wrong in specifying the pref value = 0 in tne fvSolution file, right?
Right, since you're solving for incompressible flows. As long as you do not over-specify the boundary (setting p and U at the same side, for example), it will be fine. The only difference could be a translation of the values of p.

Quote:
when I am using a steady state case, do I have to clearly enter "nCorrectors" as 1, or by default it takes as one inside?
Yes, the dictionary entry is required.

Quote:
what is the value given for "nNonOrthogonal Correctors" for a tetra mesh?
It depends on the mesh quality. Use checkMesh. If the skewness is OK, you probably do not need correctors. If the skeweness is high, you need them. The generally suggested value is between 1 and 3.

Best,
Fine, sharonyue, ebrahim27 and 4 others like this.
__________________
Alberto Passalacqua

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats.
OpenQBMM - An open-source implementation of quadrature-based moment methods.

To obtain more accurate answers, please specify the version of OpenFOAM you are using.
alberto is offline   Reply With Quote

Old   June 17, 2014, 14:42
Default
  #5
New Member
 
yalong cai
Join Date: Feb 2014
Location: New York
Posts: 13
Rep Power: 3
pizicai is on a distinguished road
Hi, alberto, I have confusion about this : " setting p = pRefVal in the cell of index pRefCell."

what cell is the pRefCell? pRefCell is usually set to 0, does this mean the pressure of NO.0 cell is zero? but how come I know NO.0 cell locates at the outlet in your case?

if this question is not described clear enough to you, please tell me.

Thanks.
pizicai is offline   Reply With Quote

Old   July 19, 2014, 04:58
Default
  #6
New Member
 
Josefine Wilms
Join Date: Sep 2009
Posts: 10
Rep Power: 8
Fine is on a distinguished road
Hi Yalong

You probably figured this out by now...just in case:

An alternative to pRefCell is to specify pRefPoint i.e.
pRefPoint (0 0 0);

Or, if you want to specify pRefCell you can open your grid in parafoam. In the menu go to Edit and then go to "Find data". There you can enter the cell ID as 0 and it will be displayed on your mesh with a coloured dot.

Set your view in paraFoam to solid colour and surface with edges...then you can see the cell more clearly

good luck
f
Anne Lincke likes this.
Fine is offline   Reply With Quote

Old   October 21, 2014, 00:32
Question
  #7
Senior Member
 
maysmech's Avatar
 
Join Date: Jan 2010
Posts: 347
Blog Entries: 2
Rep Power: 9
maysmech is on a distinguished road
Hi all,
In a fluidized bed which the top is set zero constant pressure, it is predicted to have positive pressure in the inlet, because of pressure drop in the direction from inlet to outlet. the mean time averaged of pressure is positive in inlet but the instantaneous pressure fluctuates between large positive and large negative values from time step to time step.
I saw this trend in many solvers like pisoFoam, DPMFoam, ... which the instantaneous pressure (P) sign is not similar to what we predict. Again, This is for cases which we set outlet as constant pressure. Any idea?
maysmech 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
Calculation of the Governing Equations Mihail CFX 7 September 7, 2014 06:27
specify a reference pressure point in FD method? Rui Main CFD Forum 10 August 30, 2010 08:50
Domain Reference Pressure and mass flow inlet boundary AdidaKK CFX 12 February 11, 2010 21:28
RE: Reference Pressure dilemma CFD USER CFX 7 September 3, 2008 07:51
Changing reference pressure Andrea CD-adapco 3 May 15, 2008 18:20


All times are GMT -4. The time now is 09:25.