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

FLUENT porous zone inputs

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 26, 2012, 11:28
Default FLUENT porous zone inputs
  #1
Member
 
Join Date: Jun 2011
Posts: 48
Rep Power: 6
eishinsnsayshin is on a distinguished road
Hello,

I'm trying to model a condenser and radiator as porous zones in a fluent simulation. My mesh is made in ANSA 13.2.3. I have named the volume and property ID for these zones as different things in ANSA. This means that in FLUENT, my radiator for example, has both a cell zone called "radiator volume" and a boundary condition zone automatically created called "interior-radiator volume".

My question comes with the inputs for porous zones. If you're setting an interior zone in the "boundary conditions" tab to be a porous zone, you simply input your alpha (periability of medium), medium thickness, and your C2 coefficient (pressure jump coefficient). So I did that. With setting a cell zone to a porous zone however, you go to the "porous zone" tab in the cell zone conditions menu and enter your alpha and C2 for your 3 direction vectors. My question is that alpha in this tab has units of (1/m^2) instead of (m^2). So in this menu, is the alpha input really a 1/alpha input? But in the Boundary Conditions area you actually enter regular alpha? Is that correct? Why would they do this? The C2 input is the same for both set up menus.

Secondly, Should I only enter in porous zone inputs for one of the zones (not both for a cell zone condition and boundary condition)? I'm guessing that cell zones are created for only the volume elements created during the meshing process, while automatically created "interior" boundary conditions are created for the boundary of such a cell zone.

Thanks for any explanations!!
eishinsnsayshin is offline   Reply With Quote

Old   November 27, 2012, 09:45
Default
  #2
Senior Member
 
Vangelis Skaperdas
Join Date: Mar 2009
Location: Thessaloniki, Greece
Posts: 163
Rep Power: 9
vangelis is on a distinguished road
Hi there,

Indeed permeability is usually measured in m2 units
the so called Darcy or viscous pressure drop coefficient.

In Fluent however they seem to have it defined as 1 over permeability.
So just enter the inverse value ( I guess this is a very high number)
and it will work well.

The inertial or Forcheimer term is expressed in 1/m.

About your second question you are right, ANSA Volume PIDs
are expressed as Cell Zones in Fluent where you specify if they
are fluid, solid or porous or MRF.

Interior Boundary conditions are "transparent" to the flow internal
boundaries between different Cell Zones

Vangelis
vangelis is offline   Reply With Quote

Old   November 27, 2012, 10:48
Default
  #3
Member
 
Join Date: Jun 2011
Posts: 48
Rep Power: 6
eishinsnsayshin is on a distinguished road
Hey, Thanks for the reply,

So for the interior BC's created by FLUENT between, for example, my radiator and surrounding fluid cells, I should just leave it as an interior zone, and not create a porous-jump BC in the BC panel?

Thanks!
eishinsnsayshin is offline   Reply With Quote

Old   November 27, 2012, 10:55
Default
  #4
Senior Member
 
Vangelis Skaperdas
Join Date: Mar 2009
Location: Thessaloniki, Greece
Posts: 163
Rep Power: 9
vangelis is on a distinguished road
u r welcome,

Yes, do not create a porous jump in that interior zone.

This is to model something very thin, like the pressure
drop from a thin grill for example.
In your case you have the 3D representation of your porous zone
vangelis is offline   Reply With Quote

Old   November 27, 2012, 10:59
Default
  #5
Member
 
Join Date: Jun 2011
Posts: 48
Rep Power: 6
eishinsnsayshin is on a distinguished road
Excellent thanks!
eishinsnsayshin is offline   Reply With Quote

Old   December 19, 2012, 09:20
Default
  #6
New Member
 
rayolau
Join Date: Aug 2012
Posts: 23
Rep Power: 4
rayolau is on a distinguished road
Hi everyone!

I hope you can help me, I see that are expert in porous fences.
If my wall has a height of 3 meters and I want to have a 50% porosity, in boundary conditions, I put porous jump, what I have to enter values ​​in
- Face permeability (m2) ??
- Porous medium thickness (m) ??
- Pressure jump coefficient (1/m) ??

My model is in 2D.

Thanks in advance!
rayolau is offline   Reply With Quote

Old   December 19, 2012, 09:33
Default
  #7
Senior Member
 
Vangelis Skaperdas
Join Date: Mar 2009
Location: Thessaloniki, Greece
Posts: 163
Rep Power: 9
vangelis is on a distinguished road
I believe the equation for pressure drop is:

Pressure drop= viscosity/permeability*U*[porous medium thickness] +0.5*porous jump*U^2*[porous medium thickness]

But you should better check the manual

You need to find data maybe for perforated plates in order
to find values for permeability and porous jump coefficients.

Your input should be porosity (open to overall area) and plate thickness

hope this helps

Vangelis
vangelis is offline   Reply With Quote

Old   July 11, 2013, 10:10
Default
  #8
Senior Member
 
Tanjina Afrin
Join Date: May 2013
Location: South Carolina
Posts: 158
Rep Power: 4
Tanjina is on a distinguished road
Hi Vangelis,

Could you please tell me how can I calculated Face permeability for Perforated plate ? And should I put any porosity in cell zone condition for perforated plate ?

Any suggestion will be really helpful for me . Thanks
Tanjina is offline   Reply With Quote

Old   July 11, 2013, 10:35
Default
  #9
Senior Member
 
Vangelis Skaperdas
Join Date: Mar 2009
Location: Thessaloniki, Greece
Posts: 163
Rep Power: 9
vangelis is on a distinguished road
Hi Tanjina,

You may find some references in
Perforated plate

google for some more I guess.


If it is a perforated plate better model it with a porous jump not a porous cell zone with thickness, unless the thickness is significant.

Hope this helps

Vangelis
vangelis is offline   Reply With Quote

Old   July 11, 2013, 10:53
Default
  #10
Senior Member
 
Tanjina Afrin
Join Date: May 2013
Location: South Carolina
Posts: 158
Rep Power: 4
Tanjina is on a distinguished road
Thank you very much for your prompt reply. I am very new user of fluent. thats why my questions seem to stupid to you. I am sorry for that.

This thread was helpful. Actually I wanted to model a porous pipe submerged in water (2D) So I assigned a BC for pipe in porous jump. But couldn't find out how can I assign alpha value. After reading user guide, found some formula which gives me negative alpha value ! ( Fluent user guide 6.3, article 7.19.6).

Then i thought whether can i model the pipe as a perforated pipe. But couldn't find out a way that how can I model a pipe as a perforated in 2D using workbench.

So my question is how can I model the pipe as a perforated pipe? Should I Just use the porous jump BC? If yes, then what value should I put for alpha ?

I am sorry for ling thread.
Tanjina is offline   Reply With Quote

Old   May 11, 2014, 02:20
Default
  #11
New Member
 
jody
Join Date: May 2014
Posts: 2
Rep Power: 0
fluent_20 is on a distinguished road
Hi. I want a plate devide to 3 porosity media. from up to down for
2m high 50% porosity and 3m high 20% porosity and 1m high 10% porosity.
How I do mesh in gambit and condition boundary in fluent?
Thanks
fluent_20 is offline   Reply With Quote

Old   May 11, 2014, 23:26
Default
  #12
New Member
 
Junphy Liues
Join Date: Apr 2014
Posts: 9
Rep Power: 3
Junphy is on a distinguished road
Quote:
Originally Posted by fluent_20 View Post
Hi. I want a plate devide to 3 porosity media. from up to down for
2m high 50% porosity and 3m high 20% porosity and 1m high 10% porosity.
How I do mesh in gambit and condition boundary in fluent?
Thanks
mesh has nothing to do with the porous or not, this is just the setting when you do the calculation.
Junphy is offline   Reply With Quote

Old   May 12, 2014, 06:14
Default
  #13
New Member
 
jody
Join Date: May 2014
Posts: 2
Rep Power: 0
fluent_20 is on a distinguished road
someone said me :You can define 3 different fluid zone in your gambit file. So, you have the option to put different porosity for each zone.Is that right?
setting different porosity I must do in an interior zone in the "boundary conditions" tab to be a porous zone?
fluent_20 is offline   Reply With Quote

Old   September 9, 2014, 11:30
Default porous zone confusion
  #14
Member
 
hashim chaudhry
Join Date: Jun 2014
Location: turkey
Posts: 44
Rep Power: 3
chaudhry_hashim is on a distinguished road
Send a message via Skype™ to chaudhry_hashim
Hi all, I am working on fan simulation in a duct in order to get fan curve so I created a porous region at the end of duct to introduce some reistance. what I did I just created a porous zone in which I gave the values of relative velocity resistance formulation (viscous resistance) and inertial resistance in all three direction, for fluid porosity I put the value of 1 considering the flow is fully chocked.
My geometry is cylinderical so should tick the conical box in the porous zone and as from above discussion I understand that I should not have to use the porous jump BC at the interior of porous region. Do coorect me if I am wrong ?

Thanks in advance

Last edited by chaudhry_hashim; September 10, 2014 at 03:40.
chaudhry_hashim 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
Mesh conversion problem (fluent3DMeshToFoam) Aadhavan OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 1 December 12, 2012 11:38
Modelling flow thru wet porous media in fluent???? Abhya FLUENT 0 September 2, 2012 02:59
Porosity profile, dividing a zone, or getting zone location from zone khoopes FLUENT 0 June 2, 2012 19:39
[ICEM] Export ICEM mesh to Gambit / Fluent romekr ANSYS Meshing & Geometry 1 November 26, 2011 13:11
Inputs for porous zones in FLUENT Roel van Os Main CFD Forum 1 September 1, 1998 12:41


All times are GMT -4. The time now is 05:12.