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

setting pressure gradient in the internal field

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   January 15, 2015, 19:01
Default setting pressure gradient in the internal field
  #1
New Member
 
ahmad
Join Date: Oct 2012
Posts: 5
Rep Power: 13
afaizm is on a distinguished road
Hi guys. Can anyone explain how I can set the pressure gradient as the initial condition in the internal field?

Most studies use pressure gradient as their initial condition to drive the flow in the streamwise direction. I'm trying to do the same using pisoFoam.

I would appreciate any suggestions. Thanks.
afaizm is offline   Reply With Quote

Old   January 16, 2015, 17:08
Default
  #2
Senior Member
 
Michael Prinkey
Join Date: Mar 2009
Location: Pittsburgh PA
Posts: 363
Rep Power: 25
mprinkey will become famous soon enough
If the flow is internal, you can use inlet and outlet pressure conditions to manifest your pressure gradient. The pressure field cannot just be applied as an initial condition because it will depend on potentially complicated flow behavior between the inlet and outlet. pisoFoam will solve the pressure field during its first timestep calculation and the pressure driven flow will evolve.

That is all I can offer without more details about what you are trying to accomplish. I know some simulations may use periodic domains (maybe for DNS/LES) and try to apply a pressure gradient to drive the flow. If that is what you are trying to accomplish, you can pick a pressure gradient and then add it as a source term to the momentum equation as a body force. Note that this is applicable only to simple flow domain (periodic channel flow, periodic flow between two plates) because in more complicated flow configurations, you cannot assume a uniform pressure gradient source term.
mprinkey is offline   Reply With Quote

Old   January 18, 2015, 19:58
Default
  #3
New Member
 
ahmad
Join Date: Oct 2012
Posts: 5
Rep Power: 13
afaizm is on a distinguished road
Hi Michael. Thanks for ur suggestion.

I'm running LES for turbulent flow over a surface with two rows of buildings. And, it's a periodic domain, very small with low velocity applied at the top boundary. So, within the internal domain, I wish to set constant pressure gradient, as done in previous studies as u said.

So far, I have only set uniform velocity within the internal field as the initial condition, and its value is the same as the one on the top boundary. That's pretty much summarized my boundary conditions.

But of course I will look into how I could add the pressure gradient term. This would involve compiling a new version of pisoFoam solver, which I haven't done before. Thanks again.
afaizm is offline   Reply With Quote

Old   January 18, 2015, 20:32
Default
  #4
Senior Member
 
Michael Prinkey
Join Date: Mar 2009
Location: Pittsburgh PA
Posts: 363
Rep Power: 25
mprinkey will become famous soon enough
Conceptually, replace p with p_0 + x * (p_{high}-p_{low})/L_x. p_{high} and p_{low} are the pressures on either side of the periodic BCs. L_x is the distance between the two periodic boundaries. When you insert that into the equation, you get the form for the body force. PisoFoam will be solving the flow with the modified pressure p_0. So the full pressure (for post processing) will require you to add the linear term back on by hand.

As long as your boundary conditions are only periodic or zero-gradient for pressure, this transformation is valid for any geometric configuration. Also, this assumes incompressible flow.
mprinkey is offline   Reply With Quote

Reply

Tags
internal field, pisofoam, pressure gradient

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
sonicFoam - pressure driven pipe: flow continuity violation and waveTransmissive BC Endel OpenFOAM Running, Solving & CFD 3 September 11, 2014 16:29
Moving mesh Niklas Wikstrom (Wikstrom) OpenFOAM Running, Solving & CFD 122 June 15, 2014 06:20
SPH - Finding Pressure Gradient Anywhere sckulp Main CFD Forum 0 March 13, 2013 18:14
Pressure BC for combustion chamber Giuki FLUENT 1 July 19, 2011 11:35
Implicit elliptic pressure field equation. TheBoyce Main CFD Forum 2 June 3, 2011 13:08


All times are GMT -4. The time now is 02:14.