In many of the applications I use CFD for, is orifice plates (plates with many holes for equalising the flow distribution) or/and also heating surfaces in the flow domain. It is not possible to include the orifice plates in detail, it would mean modelling of 10.000 holes and the heating surface are often tubes with fins or pins, which again would be impossible to include. The normal approach I use is a porous zone with body forces with an isotropic resistance, dp=K*u^2

Has anyone done a detailed study and compared how good an approximation the porous region with resistance is? How well is the flow distribution, pressure drop and also important the kinetic energy predicted downstream.

Thanks in advance Jan

Hmm, no responses I guess it can be due to 4 reasons

1) Nobody calculates problems with orifice plates or heating surfaces

2) Nobody cares if the approach with bodyforce represents an orifice plate well

3) People that solves problems with orifice plates has minimum 100 CPU's and just do a detailed modelling

4) I have not explained my question very well

regards Jan

Put your question on a sheet. Go to the CFX user conference. Put the sheet on the overhead projector. Make a threat that you will not leave the room untill you have an answer. We can discuss it in Strassbourg.

Maybe I need to follow your suggestion We can discuss it over a beer in Strassbourg. Have you booked a Hotel? The one I wanted was completly booked. Jan

Jan, Alas I'm not going to the conference, however should make for a very interesting section in the proceedings. No 20 pages of diagrams, figures, tables or sinopsis. Just a single Line, followed by loads of Discussion. Go for it, it should be fun !! Dave

I could be fun, I have a presentation with the title; Numerical and experimental investigation of the internal mixing of air and water in a scaled twin fluid Y-jet atomizer. That should cover it

But it would be nice if some would reply to this.

I have made a simple investigation of a problem: Orifice plate with 7x7 holes, hole diameter 60mm, porosity 60%. The inlet is placed 6 diameter (6*60mm) upstream and the outlet is placed 15 diameters downstream. (HUW scheme, no grid independant investigation) The inflow is a vulcan shape of the normal velocity and a rotating flow.

According to my handbook should the pressure drop be about 100Pa. I have used the 100Pa for calculating the resistance coefficient in the body force calculation.

Case 1 - real geometry 7x7 holes Case 2 - Resistance only depends on U^2 Case 3 - isotropic resistance ~ U^2 V^2 W^2

The static pressure difference between inlet and outlet was respectively 60Pa, 100Pa, 80Pa The maximum normal velocity at the outlet was respectively 20, 20 and 17.5 The maximum rotational velocity at the outlet was 5.6, 11.1, 4.4 The maximum kinetic energy at the outlet was 10.5 , 8.5, 5.4

The static pressure difference for case 1 seems low for case 2 it fits and also for case 3 if the dynamic pressure loss is taken into account

The normal velocity is the same for case 1 and 2 but is lower for case 3.

The rotational velocity for case 2 seems overpredicted and is probably due to the resistance only depends on the normal velocity.

The kinetic energy seem underpredicted for case 3, and also for case 2, which probably is due to that the holes generates turbulence which the prous zone does not.

If case 1 is correct then; Case 2 predict the normal velocity best Case 3 predicts the rotational velocity best, case 2 much to high. case 2 and 3 underpredicts the turbulence, much to low in case 3.

The pressure drop for case 2 and 3 is higher than for case 1, I could reduce the resistance coefficients but that would on the other make the velicities worse. I will continue my quest.