Im in the process of modelling my own ducted fan design in Fluent/Gambit. I am having an issue trying to assign the correct boundary conditions. The design is a co-axial ducted fan model. The inlet, for hover has been assumed to be a pressure inlet at 0 gauge pressure, however, since the blades are buried deep in the duct, the second set of blades is reasonably close (couple of inches) to the exit, therefore assuming gauge pressure as zero (as would be assumed in the far wake) would be incorrect. Also, options such as the using a mass flow for the exit may have be appropriate had it not been for the fact the I am vectoring part of the air which come out from the main duct, which I guesstimate, but nothing more. Does anybody have any experience with modelling ducted fans? I am using the 'Inlet fan' and 'Exhaust fan' options for now as the upper and lower fan options, which I will eventually replace by the generic fan option and add the swirl component.

Does anybody have experience with modelling airflow about helicopter blades? I know that blades can be designed and then rotated, however, that wastes my computation time due to additional elements. I am not really interested in the blades right now, just the flow in duct. Therefore, have assumed standard options of inlet fan and exhaust fans. Note that there is also an issue of defining the direction of rotation (two set of blades rotating in the opposite direction) which I am trying to model. Perhaps changing the axis of rotation from 1 to -1 will work?

Any ideas on a more appropriate model using FLUENT 6.1.22 and GAMBIT 2.1.6?

I don't use FLUENT but CFDesign for my work on this type of analysis. But i think the basic approach is pretty much the same. Since your lower fan is closed to the exit, my thought is you should not model this just as an internal flow problem, instead make it external. From what you wrote about assigning zero pressure at inlet, I think this is a static case problem. And since you also have vectored thrust at the nozzle, I just don't think having just the internal duct with the nozzle exit plane as the computational boundary exit plane can really represent what you want to model. So, create extra volume surrounding the duct. Don't make your lateral boundary too close (min r/Dfan = 20), cos in static case flow got sucked into the inlet from all over, and I won't be surprised if you see flow coming out from the nozzle recirculates back to inlet. One more thing, since now you are not putting the blade CAD into the model but just using the fan options, then you don't need to worry too much about the tip clearance issue. But in the future, when the real blade model is in, then tip clearance will strongly impact your pressure rise across the blade.

Thank you for your response,

'From what you wrote about assigning zero pressure at inlet, I think this is a static case problem.'. Indeed that is the case I am studying. And I do get some (on convergence, not a whole lot) of flow back to the inlet.

Modelling a volume over the duct entrance and below the exit is an approcah I had thought off. However, the problem is assigning the boundary conditions to the surfaces between them. I'm finding it difficult to assign the boundary condition at these zones. For example: I am considering the half model of a circular duct which has inlet as gauge pressure and therefore if i were to add a semi-circular volume over my inlet, it would not make a difference because the pressure at the inlet of both the new volume and the main duct section is 0 gauge.

If I were to have extra volume surrounding the main duct walls, would it make any difference? Cos the walls are assigned as 'wall' anyways. The tip clearance has to very very small so as to prevent the re-circulation of fluid and tip going supersonic, and that would allow me to use the entire blade ( one of the major benefits of using ducted fans). However, the good news is, I can specify the pressure increase over the fan section using the fan option. Therefore, I calculate the pressure rise from thrust required and disc area. Therefore, I have a polynomial increase of tangential velocity along the radius and a radial component and the pressure rise I can specify too (Giving me a more accurate model than I had hoped)

I used the 'Outflow' boundary condition for both my outlets (since I do not know the pressure or velocity) of either of the outlets. I believe it works by assigning the appropriate mass flow as per area to each exit (which works just fine). Any suggestions on which boundary conditions I would use if I were to add another volume at the exit? (Pressure at the far wake is an attractive option, but does not work cos air isnt an ideal gas.)

I get very pretty colorful results which look practically reasonably (I cant really experimentally verify the flow, right at this moment). The pressure on the second set of blades is greater than the first, and the pressure on the outlet consequently greater. There is a small amount of recirculation which I shall attempt to address. the velocity vectors drawn per velocity look a bit suspect, but I believe eddies has much to do with it.

Do you know of any resources on the internet which give me downladable 3D models of NACA airfoils?

Sincerely, Vishu

In your 2nd paragrpah, you mentioned "finding it difficult to assign the boundary condition at these zones". My thought on this is, the air volumes need to be big and boundary are far away from inlet or nozzle exit, then you can assign zero gage pressure. It does eat up some mesh counts of course, but compared to the mesh density on the blades or in the duct, this is peanut, unless you are already running at the extreme of your memory. And When I said adding volume, I don't mean one seperate volume each at inlet and nozzle but one for all. For this layout, you won't need to worry what BC to assign between the surfaces. Back to the mesh problem, you can create different air volumes (for exapmle small air volume just covering the ducting, then a mid size volume covering to maybe r/D of 10, then a big volume to r/D of 20 or more. This will give you a more effecient mesh count. There is one important note on static case problem, the flow is sucked in from all over at static (zero gage pressure). At inlet location, there is some amount of air speed, which means the pressure at inlet is less than zero gage. And in reality you don't really know based on your nozzle design (area ratio) you will have p exit really equals p atmosphere. That's is why I prefer creating air volumes, cos there are too many assumptions on flows at inlet and nozzle exit.

Is your tip speed based on your RPM transonic or supersonic? How many blades in the prop? (Curious to know)

Would you agree with me on the notion that the prop (or fan) performance is a function of the airflow quality going into the prop. So for your most detailed run, you should physically model the prop and not using the fan option cos if your inlet flow is not as perfect as you think it is, then the prop performance is not garenteed! (this goes to the radial pressure and velocity distribution).

I get confused on your second last paragraph. Are you already modeling the problem with real blades or you are still using the fan options?

check out this website on airfoils coordinate: http://www.aae.uiuc.edu/m-selig/ads/coord_database.html

An actual model of the rotorblade would certainly be far more precise in offering a realistic solution. I couldn't agree more. The model I had made using pre-existing fan model was to get an overview of the flow in the system. Now, to begin the more elaborate work of modelling the rotating solid rotorblades using sliding meshes.

I believe I understand how you would model the volume, but the exit/outlet is a little more involved, not offering itself to being extended. What you reccomend would work just fine for the inlet though.

I believe modelling of a mixing fan seems to be an appropriate beacon(http://www.fluent.com/worldwide/swed...s_sparging.htm).

I am trying to optimize the tip speed based on appropriate transmission elements and power supply. However, I should be able to keep the tip speed below 0.8 Mach quite comfortably.

I have started with a design estimate of 3 NACA0012 blades (just because I have data from a basic analysis in 'FlightLab') in each prop. (co-axial rotor model) due to literature that three blades provide better vibration and noise characteristics than two. However, I shall use four blades in my fluent model just because it lends itself to symmetry in my half model and also to see wither there is any significant disadvantage of using 4 blades instead of three. If doesn't ofcourse, I get all the advantages of lower disc loading.

Your link was immensely helpful and I look forward to your suggestions and comments.

Sincerely, Vishu.