I am looking at trying to figure out how different protective covers affect the airflow through a fan. I am now worried about any particular environment settings, just the same fan settings in each scenario, paired with a different design set of covers. Typically these are the type of products to stop people from jamming their fingers into the blades of the fan.
I have the fan curve data for the fan I am using, and that seems to be fine, but I am looking for some advice for an ideal scenario to put the fan and covers into. At the moment I have a very simple tube effectively, the fan in the middle of the tube (no air can slip past the outside of it. Then the ends of the tube have a pressure = 0 boundary condition. So my thoughts are that the fan curve based fan material will pull the appropriate volume of air through the covers, and I should be able to compare the final CFM and spot the differences.
Is there a better way that I could do this? I am grateful for any thoughts or feedback.
Many thanks in advance.
Your setup sounds sensible and really would give you the flow rate in an open condition. From here you could start to optimise the design.
If you are looking to produce a curve, what we typically do is either run with a higher pressure or a flow rate at the outlet. CFD will predict either the lower flow rate (with increased back pressure) or back pressure with the prescribed flow rate.
We do recommend ramping the BC up over 100 iterations and the Rotating Region up over 50, so these would be transient.
Hopefully that will help.
Thanks for the info, I have been playing with a few different concepts using my original set up, and I am getting what seems like reliable results, so I am happy with my settings.
My next question is, I am wondering how I could compare this to how freely air would move due to convection. Now I know that for me to do this I would have to turn on bouyancy, and also understand what temperature difference I would use. With this in mind, rather than having my current pressure = 0 inlet and outlet, what would you recommend I use as my BCs?
Would you have a heat source (the fan) driving the flow or do you have a fixed temperature differential (I have never run natural convection with a dT but guess it could be done!).
With a heat source we would have:
Bottom face p=0 and T=ambient
Top face p=0 and film coeff = 5W/m2/K at ambient +1C (the plus one helps stabilise the plume).
(this we call the 'chimney approach')
You would also need gravity on. Use earth and a value of 1 in the downwards direction (unless not mounted on earth.. )
I guess you would also need to set the RR as free spinning.
What might be a better approach would be to run with a resistance material where the fan is, with a heat load, to establish what the flow would be, then run a forced convection with the fan in place.. just a thought.
If you are going to attempt running without a heat source, you could try replacing the film coeff with a higher temp, not sure if it would work though. Feel free to keep me informed as you progress.
Basically I am trying to get an idea for how restrictive our fan covers are, and as these fans are used to exhaust hot air from the top face of a unit, I want to gain some idea for how close we are getting to simply having a hole and not even installing a fan and letting natural convection do its job!
So I don't need to place a resistance material in place the fan or any covers, I am just going to leave the space as one continuous fluid.
I will set the base of my analysis to be the heat source, set to the T of the equipment heat sources inside the unit. I will set the T of the top face to be room ambient for now, will that work?.
I do have a couple of questions though, what are your reasons behind using a film coefficient and a p=0? Also what do you mean by RR?
Thanks so much for your help, this is a bit of weird one, I am not used to doing simulations like this so its pretty interesting!
Its been a while since I did a natural convection analysis. In the solver I checked natural/free, as Y is my vertical axis I set gravity to -1, and I made my air material variable? Do I also need to make turbulence Laminar?
I would approach this differently (with a heat source as a power load) but let's see if this works. Use a film coefficient on the top surface though, so you are setting the ambient but allowing the heat to escape at a larger rate as it heats up.
Untick natural/free - these are shortcut analyses and will not give you the full details.
Yes, Air set to variable.
Typically I use mixing length for natural convection models.
RR = Rotating Region.
So I have adapted my scenario a little more, and rather than concentrating on the fans themselves, I am looking at their effect in a larger scenario.
So I have chosen a telecommunications cabinet, so imagine a solid (assumed that there are no leaks) cabinet, inlet in place of the front door, and a bank of equipment mounted behind the door.
I have set up a number of fans in the bank of equipment, using a fan curve I created in my previous analysis. At the rear of the equipment, rather than the air being exhausted out of the back of the cabinet, I am simulating the use of solid doors and having the air travel upwards and out of a vertical duct mounted in the top of the cabinet.
My first analysis is with the duct open, with no obstruction to flow, so I can measure the CFM that the equipment moves.
The second analysis is exactly the same, but with a fan tray mounted at the base of the vertical duct, in theory to help move more air. There are a number of fans in this tray, all based on fan curves.
My theory was that if the equipment in the cabinet, had a total of x CFM when there is no obstruction, then I place a fan tray with a max CFM of y (y being less than x), then the fan tray, while being designed to help the flow, actually restricts the flow (as its capacity is less that what the equipment is exhausting).
However I seem to be proven wrong, and it seems that the addition of the fan tray seems to be multiplying the CFM exiting the system (by a factor of 4-5). Now I am willing to admit my fan theory may just be completely wrong, and what I did here was prove that adding units of fans set up as a parrallel array, in series with each other, massively improves air flow?
Or is my analysis giving me some erroneous numbers?
Interested to know any thoughts on this!
Also, another interesting thing to note. In the analysis where there is no vertical duct obstruction, the inlet CFM is pretty much exactly the same as the outlet CFM. Which is what I would expect.
The analysis with the fan tray in the vertical duct has a massive difference, the inlet according to my results isn't allowing any CFM into the system?
I am very confused as to whats going on now!
Just experimenting with my model, I placed a small hole in the plate where the fans in the vertical duct are located, and now I am back into a situation where the exhaust CFM is now below that of when there was no obstruction in the vertical duct, and the inlet and outlet CFM now match....