# perforated plate, flow direction

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

 May 29, 2013, 14:38 perforated plate, flow direction #1 Member   Benny Join Date: Apr 2012 Posts: 40 Rep Power: 6 I am struggeling with an air flow model that includes multiple perforated plates. The plates are used to smoothen the air flow. The plates have a diameter of 30mm and the plate has an hight of 15mm. Number of holes is 10000 for each plate. therefore we will use a porous model description for each of the plates. We calculated the pressure loss for different velocties for a submodel of the plate-> we get the loss coeffiecnt for the por. model. The pressure loss in the porous model works fine but the flow after the plate is not correct. Normaly the flow gets directed in the holes so that the flow tends to leave the plate more straight even the flow reachs the plate under different atack angles. If i play with the transverse streamwise loss coefficient I can bent the flow in the right dirrection but now the pressure loss is not correct compared to the "real submodel calculation". Was anybody faced with such problem and has an idea how to get close to "good" plate description? In the end we are interested in the flow distribution after the plates. Thanks in advance! Ben

 May 29, 2013, 17:19 #2 Senior Member   Edmund Singer P.E. Join Date: Aug 2010 Location: Minneapolis, MN Posts: 512 Rep Power: 12 This should not be an issue. Just use streamwise and transverse mulitplier. Use 100+ for multiplier. Your streamwise loss is just pressure loss/streamwise distance of porous media. If this is what you did, and you are saying that your Pdrop across the streamwise direction is not right, I would suggest that your coefficients that describe the streamwise direction are in error.

 May 30, 2013, 06:51 #3 Member   Benny Join Date: Apr 2012 Posts: 40 Rep Power: 6 Thanks for the reply! We did the following calculations on a "real perforated submodel" by explicitly modeling the holes. For the outer boundaries we used translational periodic bc. the bottom has an inlet with an uniform flow distribution. the outlet is an opening. 1) straight flow onto the plate while varying the initial velocity->dptot(vinitial) 2) Vary the initial flow angle while keeping the intial velocity const->dptot(initial atack angle) Then the next step was to create an "smeared out model of the plate" using a porous domain. Therefore we defined the following: a) Set the porosity b) Directional loss in the flow direction (0,0,1) c) Set streamwise loss coefficient we got out of the "real sim" above. There we only use dptot/L=coefficenct*vsuperficialČ In the first step we used "no transverse loss". By comparing the results with the "real" calculation for "straight flow" it compares very well. Second step was to change the atack angle in the porous domain calculation. But because of the "no transverse loss assumption" the flow will not be bent into the right direction straight to the hole chanel sides (it just enters and leaves with the same angle). Now we played with the transverse multiplier and found out that we have to set the value to about 2 to get a similar outflow direction like in the real calculations. So at the moment the pressure loss for straight flow onto the plate is correct even by using the transverse multiplier. But we get in trouble by using the transverse multiplier at different atack angles. The flow gets bent correctly into the direction but the pressure loss differs by a factor of 2. We tried to decouple a streamwise and a transverse coefficient from the "real simulation" but where not sucessfull. A) Do you know a straight methodoligy how to get the correct values? B) Or is this maybe a problem of the porous domain description of perf. plates? C) Is the correct absolute pressure drop over the plate essential for the flow after the plate or is it more important that the flow direction is correct? Thank you!

 May 30, 2013, 09:30 #4 Senior Member   Edmund Singer P.E. Join Date: Aug 2010 Location: Minneapolis, MN Posts: 512 Rep Power: 12 Why are you using a traverse multiplier that is that low? I would bump that up. I bet you are getting some transverse flow (even if it "looks" like it is straight) and it is contributing to your DP. (Perhaps plot V_transverse in your porous domain. Ideally it should be 0, and your multiplier should force it to head that way). When you have no angle of attack, the traverse component of the loss will inherently be 0 becuase V_traverse=0, so the multipiler will have no apperent effect. When you add angle of attack, you are using the multiplier to induce a large pressure gradient in the traverse direction to inhibit flow in that direction. Ideally this would drive V_traverse->0. I would increase your multiplier.

 May 30, 2013, 11:23 #5 Senior Member   OJ Join Date: Apr 2012 Location: United Kindom Posts: 475 Rep Power: 12 Please understand that while in real perforated plates, the velocities in the holes will be locally accelerated, which then reduce to the bulk values after perforated sheets; the porous zone tries to model the pressure gradient to have a energy loss equivalent to what would be in the real case. Hence, you would be too optimistic if you expect the same velocity profiles as that in real. Hence I would try to make sure that the pressure distribution is addressed more correctly. Your transverse multiplier will be the same for any angle of attack, since it is a representation of the transverse loss coefficient! And the multiplier should be typically larger ~1000, as Edmund proposes. The documented procedure for extracting the exact coefficients by simulating the angled flow on perforated plates is scarce, due to the nature of the definition of perforated plates as a porous zone, as you guessed. However whatever little I have come across, they mention that upto 30 deg to the normal angle, the normal coefficient for perforated plates remains stable, and as the angle increases beyond that, the coefficient increases rapidly. OJ

 May 30, 2013, 12:45 #6 Member   Benny Join Date: Apr 2012 Posts: 40 Rep Power: 6 Thanks for the many ideas! But I am wondering about the hight transv. multiplier. I am using only a loss coefficient. There is no permeability (~v) included. The CFX help says that by using the transverse multiplier in this case, the transverse losscoefficient will be the product of the multiplier and the streamwise loss coefficient. In my case (multiplier:2) this means that the transverse losscoefficnet will be 2 times the streamwise coefficient. CFX will then solve the equations for the streamwise and the transverse direction. Especially for higher inclination angles the transverse component will get dominant. If I will use an arbitary high value of about 1000 my transverse pressure drop will get unphysically high. Am I misunderstanding anything here? Thank you

 May 30, 2013, 13:27 #7 Senior Member   Edmund Singer P.E. Join Date: Aug 2010 Location: Minneapolis, MN Posts: 512 Rep Power: 12 Yes, you are missing the velocity term. As you said: dptot/L=coefficenct*vČ You want a big coefficient for the traverse direction. In the presence of an actual velocity in the traverse direction, the pressure drop will be high. BUT, a high traverse pressure drop will retard the flow in that direction, (naturally lowering the pressure drop). All of this tends to drive v_traverse to 0. This is the same methodology to straighten a flow.

 May 30, 2013, 14:40 #8 Member   Benny Join Date: Apr 2012 Posts: 40 Rep Power: 6 Ah! YES! I forgot abot the recursive effect of pressure drop and velocity bending! So to summerize in my words: By increasing the transverse pressure loss coefficient the velocity vectors get bent into the streamwise direction more rapidly over the height of the porous domain. So in the end there will be no more contribution of transverse loss if the velocity vectors in the first nodes of the porous zone are already in streamwise direction. This means that by increasing the transverse multiplier I should get closer to the pressure loss I expect (straight flow onto the plate). Hope I got everything!? Please let me know if i still did not catch it. Otherwise I will give it a try and increase the multiplier in my "Porous model" while simultaneously observing the pressure loss. Thank you!

 May 31, 2013, 04:39 #9 Senior Member   OJ Join Date: Apr 2012 Location: United Kindom Posts: 475 Rep Power: 12 Yes, it sounds right. However, be aware that this formulation is valid for thicker perforated sheets. For thin ones, the deviation in angle of flow past the perforated sheet won't be significant, ie flow may not always escape perpendicular to the sheet, and hence it may be worthwhile to consider simple porous jump model to simulate this. Do let us know about your results. OJ

 June 3, 2013, 16:36 #10 Member   Benny Join Date: Apr 2012 Posts: 40 Rep Power: 6 Today I did multiple simulation with the porous domain and multiplier of 1000. Result is that the vectors get bent straight and we get the pressure loss we expect from detailed simulation for "straight" flow anto the plate. Thanks everybody for the hint! BUT.... The perforated plate will have multiple different inclination angle of the flow. Therefore I expect (and detailed simulauation shows) that we have an cos(theta)^m dependence of the pressure loss coefficent. Now I am thinking how to implement this dependence into the porous domain. Sure I have acess to the flow angle onto the plate but cfx will set the "differential pressure loss" and the flow in the porous domain will have a straight flow. One needs to look for the angle of flow on the fluid side of the interface to the porous domain and set the total pressure loss in dependence of velocity and angle. This sounds easy but... Maybe has anybody a more effective way of doing this? Thanks.

 August 2, 2013, 07:33 #11 Senior Member   OJ Join Date: Apr 2012 Location: United Kindom Posts: 475 Rep Power: 12 Hello Benny, Since I am performing similar simulations, I was curious about few thing. Were you finally able to decide how to define the transverse losses? Besides, while modelling the real perforated sheet submodel with flow incoming at an angle, you must have used the periodic BCs at all four sides of the submodel? How much was the increase in resistance coefficient with different angles as compared to the normal flow? Thanks, OJ

 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 Thilo OpenFOAM Verification & Validation 0 July 3, 2012 05:29 farocean97 Main CFD Forum 0 September 12, 2011 10:57 sosososo1114 FLUENT 9 August 31, 2011 01:33 Axel Rohde Main CFD Forum 1 November 19, 2001 13:19 Adrin Gharakhani Main CFD Forum 13 June 21, 1999 05:18

All times are GMT -4. The time now is 19:17.