# PERFORATED PLATES

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

 February 11, 2000, 10:52 PERFORATED PLATES #1 María Elena Rodríguez Guest   Posts: n/a Hi, I need some guidelines to model a perforated plate. The flow throught the plate is not perpendicular. Is the boundary condition: Porous Jump a good way of modelling the perforated plate. Thanks in advance Elena Rodríguez

 February 11, 2000, 11:41 Re: PERFORATED PLATES #2 Kai Kang Guest   Posts: n/a I never done that, but if you know the permeability (porous ratio) that could be the choice...

 February 11, 2000, 14:01 Re: PERFORATED PLATES #3 LW Guest   Posts: n/a I had simulated a series of perforated plates using Porous Jump BC. You need to define the drag coeff. and/or intertial coeffi. based on the offline calculations from %opening, etc. We got reasonable results on pressure losses. But flow distributions seemed not quite confirming the testing results. Fluent might over-predict non-uniformity.

 February 14, 2000, 11:48 Re: PERFORATED PLATES #4 Volker Pawlik Guest   Posts: n/a Hello Maria Elena, there was a poster presentation on the users group meeting 1997 concerning the modeling of perforated plates inside a filter (by Andea Strehlow, Apparatebau Rothmühle. The author tested the porous jump and the porous medium model and came to the conclusion that the porous jump led to very bad results whereas the porous medium results can describe reality depending on the resistance constants perpendicular to the main flow direction. Those constants had to be vaildated by experiments. The standard advice to take the half of C1 for the two perpendicular resistance constants did not lead to sufficient agreement with reality. ..

 February 14, 2000, 14:51 Re: PERFORATED PLATES #5 Sandeep Abhyankar Guest   Posts: n/a Porous jump is really a 2-D idealisation of a 3-D phenomena. So if your have a situation in which your flow is exactly perpendicular to the porous media..the use of porous jump would be justified instead of using " porous media". But if you suspect that in your simulation the flow is really not perpendicular to the porous jump face, i would advise using " porous media model" with appropriate resistance coefficients. Especially if you have highly anisotropic porous media , with flow not perpendicular to the porous medium, then it screws up the results even further.

 February 14, 2000, 14:53 Re: PERFORATED PLATES #6 Sandeep Abhyankar Guest   Posts: n/a Refer " HANDBOOK OF HYDRAULIC RESISTANCE " (by I.E. Idelchik) , it has good details about modeling flow through perforated plates.

 February 15, 2000, 04:13 PERFORATED PLATES. POSTER R. '97. #7 María Elena Rodríguez Guest   Posts: n/a Hello Volker, Where can I find information about this 'poster representation'- (users group meeting '97 )-? Thanks in advance Elena

 February 15, 2000, 04:31 Re: PERFORATED PLATES. POSTER R. '97. #8 Volker Pawlik Guest   Posts: n/a Hello Maria Elena, you can contact the German fluent office in Darmstadt: Mr. Jirka mj@fluent.de or Mr.Löffler RL@fluent.de. Maybe they can send you a colored copy of the of the poster. What I have to admit: It is written in German. So maybe it is more or less worthless for you. .

 April 29, 2013, 03:05 #9 New Member   Tobias Join Date: Apr 2013 Posts: 12 Rep Power: 5 Hello, I have the same problem as Elena. I have a perforated plate but not a normal flow through the plate it is rahter a tangentil/parallel flow. Does anybody have a guidelinbe on this topic for modeling it in Fluent? I tried to write the people from fluent as suggested in previous comments but these emailadresses are not working anymore. I also had a look in Idelchiks Handbook of hydraulic resistance, but I only found stuff related to a normal flow through a perforated plate. Many Thanks, Tobias

 April 29, 2013, 05:22 #10 Senior Member   OJ Join Date: Apr 2012 Location: United Kindom Posts: 475 Rep Power: 12 The only chance you have got is to select a small symmetrical element of perforated sheet with few holes, and simulate at your angle to find out the resistance coefficient. This you can further use in FLUENT to model, either as porous jump or momentum source. OJ

 April 29, 2013, 08:47 #11 Super Moderator     Maxime Perelli Join Date: Mar 2009 Location: Switzerland Posts: 3,145 Rep Power: 32 Is there any possibility to build and mesh your model with perforated plate? __________________ In memory of my friend Hervé: CFD engineer & freerider

 April 29, 2013, 09:04 #12 New Member   Tobias Join Date: Apr 2013 Posts: 12 Rep Power: 5 Thank you for your replies. I acutually would like to avoide that because my plate will contain somehting like 20000-30000 holes, which would create a lot of work, especially if I want to compare different shapes of perforated plates. Thats why I thought the porous media model is a good option. I figured out how to calculate the resistance coefficient for my plate with the correlations from Idelchik. But for me it looks like that these values are only appclicable for a normal flow through a perforated plate. If I am now using a porous media model from fluent. I need to specify three different coefficients, for all three directions. And my problem is that I do not know how to convert my normal direction coefficient to the other two or hw to calculate the other two coefficients. Regards, Tobias

 April 29, 2013, 09:05 #13 Senior Member   OJ Join Date: Apr 2012 Location: United Kindom Posts: 475 Rep Power: 12 Wouldn't this be computationally extremely expensive? Even the mesh independence study will require significant time and effort! OJ

 April 29, 2013, 09:10 #14 Senior Member   OJ Join Date: Apr 2012 Location: United Kindom Posts: 475 Rep Power: 12 If you are happy to use "porous jump", then only one coefficient (C2) needs to be specified, which can be easily calculated from the value of Idelchik OJ

 April 29, 2013, 09:29 #15 Super Moderator     Maxime Perelli Join Date: Mar 2009 Location: Switzerland Posts: 3,145 Rep Power: 32 I never used Porous Model, but I thought (maybe wrong), that it was not the right choice if you want to compute the pressure drop through the perforated plate, especially if you want to compare some designs (shapes). Please give feedback how you handle your shape's comparison __________________ In memory of my friend Hervé: CFD engineer & freerider

 April 29, 2013, 09:47 #16 New Member   Tobias Join Date: Apr 2013 Posts: 12 Rep Power: 5 Regarding the time and effort I totally agree you OJ, that's why I would like to avoid modelling the plate and creating the mesh. As far as I understand it the porous jump model can only be used for a normal flow through the plate because it is only a 2D model and therefore you cannot specify any losses in the other two directions, but I would say you get these losses definitly in a case of a non normal flow over the plate.. It is even specified in the fluent manual that you can use either porous media or porous jump (for a 2D problem) for e.g. modelling perforated plates. Regards, Tobias

 April 29, 2013, 10:00 #17 Senior Member   OJ Join Date: Apr 2012 Location: United Kindom Posts: 475 Rep Power: 12 Indeed, and hence I used the prefix "if you are happy to use" In case if you aren't happy, you could use the 3d porous model. Since perforated sheet doesn't have any flow in transverse direction (through the plate) you can safely take the coefficients for transverse directions as very large O(1e5), with the coefficient in flow direction as the one arrived at using some mathematics with Idelchik's coefficient. I think you need to convert the Idelchik's coefficient into a coefficient for 100% open area. FLUENT documentation provides many methods to do this conversion. OJ

 April 29, 2013, 11:12 #18 New Member   Tobias Join Date: Apr 2013 Posts: 12 Rep Power: 5 Yes I found that example but the Idelchik values are also based on the flow of an 100% open area so just need to divide them by the thickness. I will give it a try with large values for the transverse directions, is that procedure based on something or is it just a recommendation from you? Thanks Tobias

April 29, 2013, 11:53
#19
Senior Member

OJ
Join Date: Apr 2012
Location: United Kindom
Posts: 475
Rep Power: 12
Quote:
 Originally Posted by tobiley Yes I found that example but the Idelchik values are also based on the flow of an 100% open area so just need to divide them by the thickness.
I think I would disagree. Idelchik's values are based on the the given percentage open area, thus giving us the loss coefficient for that open area, ie the ratio of dynamic to static head. Since cells in mesh that FLUENT uses are 100% open, you'd need to convert this loss factor into the value (C2) for 100% open area and then divide my the thickness to arrive at coefficient for momentum source used in the momentum equations.

Quote:
 Originally Posted by tobiley is that procedure based on something or is it just a recommendation from you?
FLUENT's only tutorial on porous media recommends this approach, wherein the resistance coefficient in the direction where the flow is not intended is set as 1000 times the flow-through value. I suggested 1e5 in transverse direction where flow can't happen, for being even on a safer side.

OJ

April 30, 2013, 00:08
#20
Senior Member

Stuart Buckingham
Join Date: May 2010
Location: United Kingdom
Posts: 267
Rep Power: 17
Quote:
 Originally Posted by oj.bulmer If you are happy to use "porous jump", then only one coefficient (C2) needs to be specified, which can be easily calculated from the value of Idelchik OJ
Last time I used porous jump, I had to specify Forcheimer and Darcy coefficients. How are you doing it with one single coefficient?
__________________
http://bc247.wordpress.com

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post franzdrs Main CFD Forum 15 August 28, 2015 00:33 Sanyo CFX 6 October 8, 2010 01:25 Mike FLUENT 0 August 21, 2007 04:16 andrew FLUENT 1 May 8, 2004 09:51 Bill Gretta Main CFD Forum 1 November 11, 1998 05:56

All times are GMT -4. The time now is 16:16.