Mass flow rate prediction of Purge control valve using set pressure drop
 

Hi,

Am working on Purge control valve optimization using CFD. Please find attached the image for understanding of flow path and structure. My customer specifications read that the valve should operate at Pressure drop of 600 hPa for a maximum flow rate of 10 kg/hr. The problem is that we don't know either inlet pressure or outlet pressure. So i used CFD to predict the inlet pressure using mass flow rate of 10 kg/hr at inlet and outlet static pressure as 10 KPa (assumed) with ref. pressure =1 atm. But i get the following answers:

Inlet static pressure (areaAve) = 187.615 KPa
Outlet static pressure (areaAve) = 10.349 KPa . Pressure drop of 177 KPa is predicted which is incorrect. Inlet and outlet pressures could be anything but we need to maintain constant pressure drop of 60 KPa for which 10 kg/hr flow rate is expected which seemed to be impossible. Any suggestions would be highly appreciated. Could not attached the image as the file size exceeds the forum limit.

There is no image of your domain, can you repost it? Few quick suggestions:

1) Make sure you have extended inlet and outlet so that the boundary conditions do not influence the physics of your domain.

2) The pressure drop should (generally) not be taken immediately across the valve but away from it. Because this is the zone where the pressure is recovering. The general recommendation is 4D upstream and 6D downstream, but it is wise to plot pressure along the axis and select the points, ie, upstream at the point where the pressure starts dropping because of valve, and downstream at the point where the pressure has recovered. Taking pressure drop immediately across the valve will result in overpredicted pressure drop (and an incorrect one if you are using it for losses and while deciding pumping requirements etc).

Hi oj.bulmer,

That's absolutely right. I've checked extending the domain inlet and outlet for other designs but it caused very less change in pressure drop value. However I will recheck the domain extension on current design. Please find attached the fluid volume image. Fluid conditions : Air @ 25 C, No heat transfer and High resolution solving scheme. If I use Air ideal gas, the solution doesn't get converged.

Well, the extensions what I see there don't seem sufficient. Typically, you would want a sufficiently long inlet pipe for a fully developed flow before it reaches the valve (or you can prescribe the velocity profile at inlet and keep the inlet a bit short) and also sufficiently long outlet pipe so that there is room for pressure recovery.

The pipe lengths preliminarily can be determined by the following formulae:

Laminar: L/D = 0.06 Re
Turbulent: L/D= 4.4 Re^1/6

D being diameter and L being the length.

That said you can make sure you have got the correct lengths by plotting velocity along the axis of the pipe and ensuring it is flatter at before it reaches valve in inlet pipe and before outlet in outlet pipe.

Of course other than this, you need to make sure you set the physics correctly (turbulent model, discretization scheme, mesh independence) when you hope for the best results.

Thanks for your inputs. Do you refer to Flow domain length or pipe extension length when you talk about L/D ratio. Hope you refer to total domain length if we know the inlet diameter or outlet diameter of valve. As you see the valve, the flow path is unstructured. Please comment.

I meant the length of the extension at both inlet and outlet. If the two diameters are unequal, you can still use the formula, except that Re will be different for both and so may L/D be. The point is to have a developed flow, which is a general practice. This will also make sure you are letting the pressure recovery to take place.

The inlet and outlet dont have the same diameter. I think you should be using total pressure difference for your drop.

@oj.bulmer,

Thanks for your quick response. Appreciate that.Will let you know the results. Is there any standard for permissible error limit in grid independence study. For instance, if i go roughly with a fine mesh, I get DeltaP=150 KPa. Then If I go further with a little refined mesh as per required physics, I get DeltaP=152 KPa. Could this difference in error be foreseen or do we have to consider it further to get almost similar results (eg: 150 KPa , 150.2 KPa...) for a better accuracy ? With reference to CFD- Wikipedia i couldn't find the answer.

@ Singer 1812, oj.bulmer
That's a nice question. In my case, inlet and outlet diameter is different. I usually measure Total Pressure difference using CFD-POST. But is it always true ? I don't think so. Why can't we measure static pressure loss with just Pressure difference using CFD-POST. Generally pressure drop or pressure difference might refer to either static or total. But this is strange. In our validation program, our testing team normally sets static pressure or gauge pressure instead of total pressure. Then how is it possible to compare the total pressure difference in simulation with static pressure loss in physical tests. Hope it makes sense. Please comment.

This depends on the extent to which you want to go in ensuring grid independence. Following is an excellent guide on arriving at the grid independence.

http://www.grc.nasa.gov/WWW/wind/val.../spatconv.html

Notice that for unstructured grid, the definition of refinement ratio is slightly different. Roache, from whose paper above guidelines come, recommends a minimum refinement ratio of 1.1 (or ratio of total no. of elements elements between two meshes be r^3 =1.33). You have to make sure that GCI for your two meshes is less than 1% etc. You can go lower or higher, depending on the extent of accuracy you want.


Edmund's concern is valid. Since the diameters are unequal, the difference between total pressure is what perhaps the best indication of the the total energy loss since the dynamic pressure will be unequal in two diameters. However, if you want to compare the results with the experimental data, you will have to use the difference between static pressure since that is what is measured by pressure gages.

In experiment, generally static pressure is easier to measure (device setup, etc...), so that is what is usually done.

If the diameters on the inlet and outlet are the same, and the flow is adiabatic, the delta static pressure will equal the delta of the total pressure.

The trouble with static pressure delta, is that you really need to match the experiment setup exactly to have the best chance of matching it and even then with a complex setup, that is not really what you want to be matching to (do a lookup on HVAC or pump static pressure vs total pressure).

You can change the static pressure delta from the experiment to total pressure via just adding the rho/2*V^2 terms to the inlets and outlets.

The link from NASA is really a good guide. I have seen this guide before but not with a detailed attention. Now its time to look at the mesh aspects. Thanks OJ. I agree with you and Edmund as I had similar understanding on pressure drop. But somehow I felt strange to compare Total pressure drop in simulation against static pressure loss in experiment though I do it all the time as control valves inlet and outlet would never be the same. Guess we don't have any other choice cause that's how the flow science is obeyed

Edmund, I use to do the same stuff. I get static pressure at inlet and mass flow rate at outlet from experiment. If I need to use Total pressure at inlet and mass flow rate at outlet, I calculate the dynamic pressure and add it to static pressure to get the total pressure at inlet. I strongly agree that matching static pressure loss in simulation with static pressure loss in experiment is very difficult. I had similar experience when I exactly tried to model the valve including the test rig setup. But still I got an error of 40% more than the expected pressure drop value.

Anyways I thought I could clarify few doubts. Thanks OJ and Edmund for participating in this post and you've really thrown some valuable comments and suggestions. Appreciate that.

Will revert back to you when i'm done with domain extension and recalculation of pressure drop. Thanks again !!!