CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   Inlet shapes for modelling a fan in an inlet duct (http://www.cfd-online.com/Forums/cfx/65171-inlet-shapes-modelling-fan-inlet-duct.html)

buzzybee June 7, 2009 03:44

Inlet shapes for modelling a fan in an inlet duct
 
I am interested to hear from people who have modelled an axial flow fan in a duct, to find out what shape of inlet they have found works best to determine the correct velocity profile in front of the fan.

In my case, I have a fan with a 2mm tip clearance placed into a duct 25 mm down from the duct entrance - see http://img218.imageshack.us/img218/7379/domain.jpg

As can be seen from this image, the domain in front of the fan is a dome shape with the 25mm of duct in front of the fan intruded and 'cut out' from the dome shape, where 1 and 2 are non-slip walls. I have been trying different combinations of inlet and outlet boundary conditions and have been getting quite different results when visualising the flow over the blades. I believe that a mass flow on the outlet and a total pressure of 0 atm (relative domain pressure is 1 atm), best physically simulates my experimental setup. However I get backflow when using these boundary conditions (with more than 60% wall off to maintain the inlet boundary condition).

As far as I am concerned the outlet is far enough away from the inlet (10 diameters, which it was in the physical experiment). I have been looking at the effect of the inlet varying the size of the dome, but would like to hear from anyone who has modelled a similar physical setup to find what shape inlet they have successfully used.

Thanks in advance for any advice/suggestions.

Jenny

ghorrocks June 7, 2009 08:14

Hi,

For an incompressible flow the inlet shape won't make much difference. For a compressible flow it might - if acoustic waves are significant then the exact location of the inlet boundary will affect how they reflect and interact with the fan. Then the shape of the inlet is vital.

You have a sharp edge just in front of the fan. That is going to cause large separations (vena contracta) meaning your fan will probably not have very even loading over the blade. This is poor fan design, but if that is what you want to model then you have to be careful to get it right. You will need enough wall section outside the pipe to have the correct velocity profile to generate the right vena contracta. This will significantly affect fan performance so could be the variations you are seeing.

Glenn Horrocks

buzzybee June 8, 2009 08:17

Hi Glenn,

Thank you for your reply. My simulation is incompressible flow, but I have been having a lot of trouble trying to get good agreement with my experimental results.

I have tried two other models:

1) http://img40.imageshack.us/img40/2497/originalmodel.jpg
2) http://img41.imageshack.us/img41/2748/model2h.jpg

The first has only 2mm between the inlet and the fan blade tips. As you say, I am getting recirculation zones from the sharp entry point into the fan. However the flow over the blades was symmetric. The flow was symmetric, but using a mass flow inlet I could not get the correct pressure (atmospheric) on the inlet dome.

The second used the same boundary conditions, but added 20 mm of duct in front of the fan, as it was in the actual experiment. Again the flow was symmetric, but the pressure not.

I feel the correct velocity profile isn't being simulated using the mass flow inlet, so tried a total pressure inlet, but then found there was reverse flow over a range of different back pressure. I then tried the model in my original post with the 20mm in front of the fan intruded into the inlet dome. Again it causes the reverse flow. Although using an opening boundary condition makes allowance for the reverse flow, this is obviously giving me an incorrect pattern of flow over the blades. Increasing the diameter of the inlet dome has helped because at least the flow is now symmetric over the blade, but this is only achieved when I use an opening.

I am at a bit of a loss what to do with the inlet and inlet boundary condition, as the duct length (10D from the back of the fan and 20mm in front of the fan), are identical to the physical experimental setup. I am therefore not sure what I can do with the inlet to give me the correct velocity profile and not create backflow.

Thanks for any suggestions.

Jenny

ghorrocks June 8, 2009 08:41

Hi,

If the fan blades are in a region of separated flow then
1) The blades will not be running very well as the tips are bound to have stalled and not be running properly.
2) Simulating a blade in the stalled condition is very difficult. You will need to be very careful to get it accurate. Probably need DES, SAS or LES.
3) I said the blade loading is uneven, not unsymmetric. I mean the centre section of the blades are running OK but the outer section in the recirculation are stalled and running poorly. This is very bad fan design. Why don't you put a bell-mouth entrance to the duct? Or move the fan back so it is away from the recirculation zone?

As for what BCs to use, how was it set up in the experiment? Just match the experimental setup. For an incompressible flow a pressure outlet and a mass flow inlet are pretty standard and should be used unless you have a good reason not to.

Glenn Horrocks

buzzybee June 8, 2009 09:36

Hi Glenn,

Unfortunately the physical experiment was set up this way and I'm just trying to numerically model the physical set up exactly as it was. The experiment was run with about 10 different pressure loads from fully open to fully closed (load was created by a plate placed at various distances from the duct outlet). With the numerical model I am using, I am getting reverse flow which is a concern to me across all pressure loads.

The assymetric flow I was talking about came when I used the model with the 20mm intrusion into the inlet dome, whereas it was symmetric using the original model with the inlet dome only 2mm from the fan blades, which seemed a bit odd.

I will try and move the fan back further down the duct, but I would have preferred to keep it the same as the physical experiment.

Thanks again for your help.

Jenny

ghorrocks June 8, 2009 18:50

Hi,

You have to model what the experiment did. If they had the fan close to the inlet then that's what you should model. But bear in mind that this is bad fan design and will make it difficult to get an accurate simulation because the fan blades will be stalled in some regions. If it is possible to get the experimental guys to redo the test with a bell mouth opening or the fan further down the duct it will not only be easier to model but also a better experiment as the results are more representative of the fan performance. At the moment the experiment is not a good reflection of fan performance and therefore it is a poor experiment.

As for what boundaries to use, how have the experimental results been presented? Again this will tell you what boundaries to use.

Glenn Horrocks

buzzybee June 8, 2009 22:37

Hi Glenn,

Unfortunately it's not possible for them to redo the experiment, but i do know there was a very small bellmouth on the inlet just to take away the sharpness of the inlet. I have tried to model this small shape, but it makes little difference. I know the experiment was set up according to the British standard, BS848 and was set up to replicate as closely as possible the real working of a small computer fan, in that the inlet is close to the fan itself.

The experiments measured the dynamic and static pressures at a distance 20cm up from the outlet. From these results I ascertained the mass flow and volume flow and plotted the static pressure vs volume flow to determine the fan's performance.

From this, I have tried to use a mass flow inlet and also a total pressure inlet, with static pressure outlet and mass flow outlet respectively. It seems like I have a complex problem, and due to the unique geometry of the fan I am testing, I am not overly confident that CFX can handle it properly to give me a believable picture of what is physically going on, since the different boundary conditions give such different solutions.

Thanks again for all your advice.

Jenny

ghorrocks June 9, 2009 08:17

Quote:

Originally Posted by buzzybee (Post 218627)
Unfortunately it's not possible for them to redo the experiment, but i do know there was a very small bellmouth on the inlet just to take away the sharpness of the inlet. I have tried to model this small shape, but it makes little difference. I know the experiment was set up according to the British standard, BS848 and was set up to replicate as closely as possible the real working of a small computer fan, in that the inlet is close to the fan itself.

OK, I see now. In that case you just have to model the geometry tested as closely as possible.

Quote:

Originally Posted by buzzybee (Post 218627)
The experiments measured the dynamic and static pressures at a distance 20cm up from the outlet. From these results I ascertained the mass flow and volume flow and plotted the static pressure vs volume flow to determine the fan's performance.

From this, I have tried to use a mass flow inlet and also a total pressure inlet, with static pressure outlet and mass flow outlet respectively.

Mass flow inlet with static pressure outlet is preferred. Have you read the section in the documentation about choice of boundary conditions? There is also a best practices guide for turbomachinery which I recommend reading.

Quote:

Originally Posted by buzzybee (Post 218627)
It seems like I have a complex problem, and due to the unique geometry of the fan I am testing, I am not overly confident that CFX can handle it properly to give me a believable picture of what is physically going on, since the different boundary conditions give such different solutions.

Yes, I agree that the system is complex but I suspect a main cause is due to the blade tips operating in a separated zone. This will cause the blade tips to stall and this can distort the flow on the remainder of the blade as well.

CFX almost certainly can model your problem, you just have not found the right way to model it yet!

Glenn Horrocks

buzzybee June 10, 2009 23:25

Hi Glenn,

Thank you again for your reply. Yes, I've read the documentation and best practices guide and have also spoken with various CFD 'experts' and even the engineers at ANSYS, and they have been recommending to use a total pressure inlet and mass flow on the outlet. They've also recommended extended the inlet duct so it is further away from the fan blades, however I want to model the real-world situation.

I agree with you about the main cause of the problem being the blade tips operating in the separated zone. Using the total pressure inlet I get quite a reasonable agreement with the experimental results, but I just can't have any confidence in flow pattern when CFX has to create a wall over nearly 99% of the inlet to keep the inlet boundary condition.

I will keep persevering, as this is a problem I have been having for quite some time now. Thanks again.

Jenny

ghorrocks June 11, 2009 06:32

Hi,

What total pressure are you using? What mass flow are you using? What fan speed are you using? Where did you get the values from?

Glenn Horrocks

buzzybee June 11, 2009 20:15

Hi Glenn,

>> What total pressure are you using?

0 total pressure with a reference pressure of 1 atm

>> What mass flow are you using? What fan speed are you using?


Mass flow ranges from 0.0083 kg/s for the setup when the plate was almost blocking the airflow coming out from the duct (i.e. the plate used to create back pressure was only 2mm away from the outlet) to 0.069 kg/s when it was almost fully open (i.e. the plate was 100mm away from the outlet). The speed of the fan was around 3600 RPM.

>> Where did you get the values from?

I have been working with another student who did an experimental study of the fan. I actually repeated the experiment last month as I was not convinced over some of the mass flow rates he had got, and was found to be correct. I had to hire the equipment, which is why the experiments can't be repeated, but I am confident with the results gained.

Update
I have been running the model with an inlet dome doubled in size, to see the effect and have run models with the dome as an inlet (Ptotal = 0) and also as an outlet (opening pressure and direction). In both cases of different diameter size, a wall was created over most of the dome area to maintain the inlet condition when the inlet boundary condition was used.

  1. For the fully loaded (2mm case), the pressure was over-predicted compared with the experimental (by 20%) using the inlet b.c and the flow looked like this within the dome:
    http://yfrog.com/5e2mminletj

    Using the opening b.c the pressure was under-predicted by 10% and the flow in the dome looked like this:
    http://yfrog.com/072mmoutletj

    The 2D streamlines over the blades in both cases are totally different.
  2. For the almost fully open (50mm case), the pressure was almost identical using either the inlet or opening boundary condition on the dome, but overpredicted the experimental value by 220% for both types of inlet boundary condition. Using the original dome diameter, which was half the size, the opening boundary condition in this case overpredicted by only 15%.

    Even though using the inlet b.c for this case, the flow looked like this in the dome - http://yfrog.com/0f50mminletj

    and this http://yfrog.com/0v50mmopeningj when using the opening b.c, the 2D streamlines on the blades are virtually the same.

I'm now experimenting with the size of the inlet a bit further,

Jenny


All times are GMT -4. The time now is 10:54.