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

Using Porous Zone to simulate an obstacle? Is it possible?

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

Reply
 
LinkBack Thread Tools Display Modes
Old   December 19, 2013, 12:50
Default Using Porous Zone to simulate an obstacle? Is it possible?
  #1
Senior Member
 
M. Montero
Join Date: Mar 2009
Location: Madrid
Posts: 112
Rep Power: 8
be_inspired is on a distinguished road
Hi all,

Maybe the aproach that I have thought is not valid but the point is this:
I have simulated a wind turbine using actuatorDisk source. Could it be possible to simulate the tower effect choosing a cellZone and impossing a very low porosity?

I am doing some tests with the DarcyForchheimerCoeffs and I can not slow down the flow as if there was a wall.
The Coeffs are: d (5e10 5e10 5e10); f (5e10 5e10 5e10)

I am not interested into the flow itself in the very near of the wall of the tower.

What I want it is a easy way to play with the wind turbine positions without the need of change the mesh itselft.

What do you think? Is it possible to do it in that way?
Thank you very much for your help
be_inspired is offline   Reply With Quote

Old   December 20, 2013, 03:28
Default
  #2
Senior Member
 
Mark Olesen
Join Date: Mar 2009
Location: http://olesenm.github.io/
Posts: 777
Rep Power: 18
olesen will become famous soon enough
Quote:
Originally Posted by be_inspired View Post
Hi all,

Could it be possible to simulate the tower effect choosing a cellZone and impossing a very low porosity?

I am doing some tests with the DarcyForchheimerCoeffs and I can not slow down the flow as if there was a wall.
The Coeffs are: d (5e10 5e10 5e10); f (5e10 5e10 5e10)
I don't see anything fundamentally wrong with your idea.
For your approach, it is important that the resistance coefficients are symmetrical (like you already have), so that an explicit porosity formulation is valid.

IMO your resistances are too low (darcy = 1e10) to stop the flow.
For comparison, an exhaust system DPF would typically have a Darcy value of ca. 3e8.

If you check the documentation, you'll see that this Darcy parameter is multiplied internally by the viscosity before being applied as a source:
Code:
S = - (\mu \, d + \frac{\rho |U|}{2} \, f) U
In your case, I don't think it makes much sense to bother with darcy/forch parameters at all - you don't actually want to model any particular resistance and you don't really care about any linkage to the fluid properties. You just want a sink that stops the flow in some relation to the velocity. In this case, the powerLaw formulation would be much, much better:
Code:
S = - \rho C_0 |U|^{(C_1 - 1)} U
You still have the density involved, but you otherwise have a fairly direct connection to the velocity. You'll need to experiment a bit, but I would start with something fairly aggressive and see if it does the trick or if it diverges. Maybe C0=1e10, C1=3?
I unfortunately have no real feeling for how far you can push the values or how far you need to push this values, but I think it is a better approach than the darcy/forch formulation.

/mark
olesen is offline   Reply With Quote

Old   December 20, 2013, 11:54
Default
  #3
Member
 
Franco Marra
Join Date: Mar 2009
Location: Napoli - Italy
Posts: 52
Rep Power: 8
francescomarra is on a distinguished road
I am not sure if this infos can be of help.

OpenFOAM already include a solver for the simulation of the presence of obstacles. You can have a look to:
$FOAM_TUTORIALS/combustion/PDRFoam
I do not know the details of this implementation, but it seems to me that it should do something similar to what you are looking for.

Best regards,

Franco
francescomarra 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
define porous zone in gambit Michel_HB OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 8 February 26, 2015 08:41
thermal porous zone dictionary Ahmed Khattab OpenFOAM 0 June 4, 2013 07:41
simulate the drying process Valpress FLUENT 6 May 24, 2013 05:27
[ICEM] Export ICEM mesh to Gambit / Fluent romekr ANSYS Meshing & Geometry 1 November 26, 2011 13:11
Porous jump & Porous zone - help needed Witsarut Jintaworn FLUENT 3 June 14, 2010 22:37


All times are GMT -4. The time now is 04:59.