# How to get a uniform showerhead?

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

May 3, 2012, 02:42
How to get a uniform showerhead?
#1
New Member

Join Date: Apr 2012
Posts: 9
Rep Power: 5
Hi, everyone. I'm simulating the flow field of a showerhead-like structure within a low pressure chamber (operated at 1 Torr). I did the work with Fluent and I already had a convergent result. However, I did not how to explain the result and might need some help from you.

Fig. 1 (see the attached file) shows the showerhead-like structure. It's basically composed of several perforated metal tubes. My main objective is to obtain a uniform gas distribution, which means the velocity at the outlet of each hole must be the same.

Fig. 2 shows the flow field inside the showerhead-like structure. As you can see, the velocity is higher near the gas inlet. At first, I expected that the velocity distribution of the holes must follow the same pattern. Nevertheless, the results showed that the velocity are identical at each hole outlet. I went back to check the pressure and found that the pressure is also uniformly distributed among the holes. I've done some research and found that the key to get a uniform showerhead is to achieve a uniform pressure inside the flow channel. I guess I can imagine the pressure as a "push force". When the pressure is uniformly distributed, the velocity at different holes would also be the same. But how to explain it in a more accurate way? What is the principle or governing equation for this phenomenon?

Moreover, I'm quite confused about the non-uniform velocity (Fig. 2) but uniform pressure distributions inside the showerhead-like structure. What is the correlation between velocity and pressure in this case?
Attached Images
 Fig. 1.JPG (66.6 KB, 31 views) Fig. 2.JPG (48.0 KB, 30 views)

 May 3, 2012, 19:13 #2 Senior Member   Julien de Charentenay Join Date: Jun 2009 Location: Australia Posts: 229 Rep Power: 9 Hi, Your explanation of the pressure force that pushes the gas (or liquid) through the hole is correct. I will rephrase it in my own words: The holes are significantly smaller than the metal tubes and therefore act as a pressure "barrier": the gas is driven through the holes by the pressure in the metal tubes that can be considered as pressure vessel. The non uniform velocity is puzzling you. The velocity plot is a plot of velocity magnitude (the velocity of the gas in the tube). At each hole, the fluid in the tube is loosing a little bit of mass to the hole (the velocity through the hole). So the quantity of mass going from one hole to the next decreases slightly up to the middle holes where the velocity is near zero. Try plotting the velocity magnitude at the center of tube from the left to the right in 2D and the velocity distribution will be close to linear. Notes: 1) the two extreme tubes are not as well served by the fluid than the middle tubes. This can be attributed to the additional pressure loss at the end corner (in my opinion). You could use a curve in place of a sharp bend to improve. 2) If you have a bit of time, you could try aligning your gas inlet with one of the tube. It will drastically change the distribution of fluid in the tube, where the tubes that are aligned with the inlet will have more fluid than the others. Hope it helps. Julien __________________ --- Julien de Charentenay

 May 3, 2012, 22:29 #3 New Member   Join Date: Apr 2012 Posts: 9 Rep Power: 5 Hi, Julien. Thanks for your reply. Your comments defenitely help a lot. Now I have a better understanding of my simulation results. I have one more questions, though. 1. If I reduce the diamater of the gas inlet tube while keep the other parameters fixed (I'm simulating gas flow. In reality, the inlet gas is controlled by a mass flow controller, which means the mass flow inlet is a constant in this case), will it help to build up a higher pressure inside the metal tube? My guess is yes. And the reason is that the pressure drop at the gas inlet tube will be higher. This will help the gas flow further into the metal tubes and improve the velocity distribution of the holes. Am I correct? Notes: 1) the two extreme tubes are not as well served by the fluid than the middle tubes. This can be attributed to the additional pressure loss at the end corner (in my opinion). You could use a curve in place of a sharp bend to improve. Thanks for the tip. It's very helpful. 2) If you have a bit of time, you could try aligning your gas inlet with one of the tube. It will drastically change the distribution of fluid in the tube, where the tubes that are aligned with the inlet will have more fluid than the others. And it will be more difficult to build up a pressure inside the metal tube. So the velocity distribution of the showerhead-like structure will be less uniform. Is that right?

 May 5, 2012, 06:48 #4 Senior Member   Julien de Charentenay Join Date: Jun 2009 Location: Australia Posts: 229 Rep Power: 9 Hi, I disagree with your guess. The driver for the pressure in the metal tubes is the size of the holes. The holes are the smaller orifices through which the gas has to flow through and will therefore control the pressure in the metal tubes. If you want a higher pressure in the metal tubes, make the holes smaller. Making the gas inlet smaller will increase the pressure drop in the gas inlet. It will result in a higher pressure at your mass flow inlet (i.e the pump will have to work harder) - but the pressure increase will be negligible compared to the pressure loss through the holes. You need to keep in mind a couple of aspects in these types of simulation: 1) The pressure level is driven by the pressure outlet. Reduce the pressure outlet by 1000 Pa and all pressures within the flow will be 1000Pa less (neglecting compressible effects if you are simulation compressible flows); 2) The CFD simulation is mass conservative. The gas you put in will go through the openings you model and only the openings you model. In real life, your tube arrangement will have seal and joint. If the pressure builds up too high, the seals/joints will be more prone to leaks. In regards to my suggestion number 2: if a metal tube is aligned with the gas inlet, the flow will dominantly go through the aligned metal tube as this will be the path of least resistance. In the model scenario, the gas inlet is facing a wall. At the wall the gas velocity will be converted into local static pressure. This ensure a "reasonable" distribution of the gas within the metal tube. My advice is: you are running CFD models. Just try and investigate (it does not cost much apart from time - this being said if you are a consultant: time is money, but so if knowledge). BTW: little tip if it takes too long to run, you can reduce the size of your case by 1/4 by using symmetry. I am happy to keep this discussion alive, but would like to get the dimension and nature of the gas so I can run simulations to improve the discussions. Kind regards, Julien __________________ --- Julien de Charentenay Last edited by julien.decharentenay; May 5, 2012 at 06:48. Reason: grammar

 May 10, 2012, 06:45 #6 Senior Member   Julien de Charentenay Join Date: Jun 2009 Location: Australia Posts: 229 Rep Power: 9 It will be a quick answer: 1) Yes, the mass flow rate will have an impact on the pressure in the tubes. Think of the pressure in the tube as a total pressure (= static pressure + velocity component). If you reduce the flow rate, the pressure in the tube will be reduced. Reduced pressure means (IMO) that it is more likely to have difference in flow rates through the holes. 2) I do not have a design guideline for you. How much would you/your company pay for one? In a nutshell, you could (by physical and numerical experience, or just aging experience) probably derive a relationship between the pressure drop through the holes and the likelihood of a bad distribution of flow through the hole - which can be easily estimated based on the mass flow rate and size of the holes. __________________ --- Julien de Charentenay

 May 11, 2012, 05:48 #7 New Member   Join Date: Apr 2012 Posts: 9 Rep Power: 5 Hi, Julien. Thanks for your kind and very helpful reply again. One more question: I ran the simulation using Ansys Fluent with imcompressible ideal gas law, which means that the pressure used to calculate the gas density is always a constant (it's the operating pressure, which is equal to 133 Pa in my case) but the temperature is taken into account. However, inside the metal tubes, the pressure is much higher than 133 Pa. I'm kind of confused about the definition of compressible gas. The definition given in most textbooks is always about the ratio of gas speed and sound speed. But inside the tube, the velocity is far much than sound speed. I think the other way to explain the compressible gas is whether the density changes. So, I should use the compressible idea gas instead to consider the influences of the pressure and the temperature. Am I right? 1) Yes, the mass flow rate will have an impact on the pressure in the tubes. Think of the pressure in the tube as a total pressure (= static pressure + velocity component). If you reduce the flow rate, the pressure in the tube will be reduced. Reduced pressure means (IMO) that it is more likely to have difference in flow rates through the holes. The explanation is very clear. Thanks. Now I got a better understanding about how the pressure is build up inside the tubes.

 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 javad814 OpenFOAM 1 September 26, 2011 13:30 Wolle OpenFOAM 2 April 11, 2011 07:32 antonio_ing OpenFOAM Running, Solving & CFD 5 September 16, 2010 02:31 claco OpenFOAM 7 April 20, 2010 04:32 kumar2 OpenFOAM Running, Solving & CFD 8 March 24, 2008 19:38

All times are GMT -4. The time now is 20:54.