[Tianyi]

Hello everyone,

I am simulating a 2D simple ducted electric fan on the aerofoil to accelerate the flow on the upper surface at high altitude (10000 m) and Mach 0.73. I am using Pressure Outlet with target mass flow rate option on for fan intake and Mass Flow Inlet as fan exit. The problem is no matter which value I set for the target mass flow rate option, the mass flow reports for fan intakes are identical. I have tried 58 and 70 kg/s for fan intake til fully converged (all residuals down to 10-4 level), however, the velocity plots for fan intake, pressure distribution plots are exectly the same. I have also checked the mass flow reports for both fan intakes, the values are the same as well (39.7kg/s), which I believe is absolutely wrong due to conservation of mass. The diameter for fan intake and exit are almost the same, just consider it as a cylinder.

Detailed BCs (settings for turbulence intensity and viscosity ratio are omitted):

Initial Condition: 26436.86 Pa, 217m/s, 223.15K

Domain Inlet (velocity inlet): 217m/s, 223.15K
Domain Outlet (pressure outlet): 0 Pa,223.15K
Fan Intake (Pressure Outlet): 27042.0 Pa (working pressure (gauge)), 223.15K, 58 and 70 kg/s (Target Mass Flow Rate option)
Fan Exit (Mass Flow Inlet): 58 and 70 kg/s recpectively, 26216.54 Pa (supersonic static pressure (gauge)), 270.16 K (total temperature)
Aerofoil and Fan Shroud are walls;
Domain top and bottom surface as symmetry planes.

The values of all pressure setting are calculated correctly (I think). Y+ is ok, boundary layer check done.

If anyone familiar with this Target Mass Flow Rate option can offer any advice, it will be much appreciated!!!

[fluid23]

I often have weird results with target mass flow option on a pressure outlet. Particularly in 2D I get odd results. Most recently my mass flow pressure outlet was acting as an inlet... don't ask me why.

I have found that simply using a mass flow inlet with negative value works fairly well compared to the target flow pressure outlet option. You can occasionally run into a few odd residual convergence issues and run times can be about 20% longer in some cases, but it seems more reliable in my experience.

[Tianyi]

Originally Posted by fluid23

I often have weird results with target mass flow option on a pressure outlet. Particularly in 2D I get odd results. Most recently my mass flow pressure outlet was acting as an inlet... don't ask me why.

I have found that simply using a mass flow inlet with negative value works fairly well compared to the target flow pressure outlet option. You can occasionally run into a few odd residual convergence issues and run times can be about 20% longer in some cases, but it seems more reliable in my experience.

Hi Fluid23,

Thanks very much for your reply, I am trying with your suggestion now. Thanks again.

[fluid23]

I believe that parameter is only relevant for a mass flow inlet with supersonic inflow... basically it will use the value you input to calculate the equation of state rather than the reference value you assigned in your physics continua. To do this, you need to know the total pressure and Mach number of the inflow then you can calculate the static pressure corresponding to those conditions from the isentropic equations, pt/ps = (1+y-1/2*M^2)^(y/y-1) where y = gamma = ratio of specific heats ~ 1.4 for air in most applications. If the flow is subsonic then the value is ignored.

For a mass flow 'outlet' regardless of whether it is supersonic or subsonic, the pressure (and temp/density) are determined by what your flow is doing. It doesn't need a user input to nail down equation of state since it is being determined by your solution already.

That being said, I would think that if you are modeling a fan inlet that the flow is already subsonic and you shouldn't worry about it in the first place. I don't think it will have any bearing on your solution, but if you are concerned you can always vary the value and see what impact it actually has.

[fluid23]

Also, if you did need to define it I would specify it as 0 not 101325 Pa. I believe that you would specify it as a gauge pressure referencing your reference pressure in the physics continua rather an absolute pressure value. If your ref pressure is 101325 Pa and you specify 101325 Pa it will actually use 101325 + 101325 = 202650 Pa.

[Tianyi]

Originally Posted by fluid23

Also, if you did need to define it I would specify it as 0 not 101325 Pa. I believe that you would specify it as a gauge pressure referencing your reference pressure in the physics continua rather an absolute pressure value. If your ref pressure is 101325 Pa and you specify 101325 Pa it will actually use 101325 + 101325 = 202650 Pa.

Hi Fluid23,

The explaination is brilliant, I really appreciate that. I have tried the method you suggested, however, I got some odd velocity contour and vectors, please take a look at the attached images if you are free to do so. Thanks.

Velocity vector plot:
https://drive.google.com/file/d/1iMF...ew?usp=sharing

Velocity contour plot:
https://drive.google.com/file/d/1wN0...ew?usp=sharing

As you can see, the both mass flow inlets (intake with negative value and exit with positive value) does not accelerate the flow which they are supposed to do, actually they both slow down the flow. The free stream velocity is 0.725 Mach, and I am pretty sure that the value of mass flow rate were set -58kg/s and 58kg/s for fan intake and exit respectively. One thing I need to mention is I am simulating the fan exit to be "just chocked" condition to maximum the efficiency. Therefore, the supersonic static pressure for intake and exit are both -28485.68 Pa (gauge) just incase the flow would be supersonic, I understand that the fan intake velocity won't be sonic anyway.

Previously, I was using Velocity Inlet to simulate the fan exit, but eventually I realised I can not have control of the fan exit mass flow as it should be identical to fan intake.

[fluid23]

Now that I have seen your application/geometry, I would recommend a different approach. The method I have described works better for an embedded engine. You have an immersed ducted fan. I’ll send you a more detailed response with a image of a typical geometry that I apply this approach when I get in the office later.

However, your solution would be better served by the use of either a fan interface or momentum source. There are several options available depending on how much you know about your fan. My brain hasn’t booted up yet this morning, so I can’t remember the name of the model just yet, but my personal favorite is a fan source which couples blade element momentum theory into a momentum source to approximate the effect of real fans on your domain.

I’ll do some digging when I get to the office and give you a better answer.

[Tianyi]

Originally Posted by fluid23

Now that I have seen your application/geometry, I would recommend a different approach. The method I have described works better for an embedded engine. You have an immersed ducted fan. I’ll send you a more detailed response with a image of a typical geometry that I apply this approach when I get in the office later.

However, your solution would be better served by the use of either a fan interface or momentum source. There are several options available depending on how much you know about your fan. My brain hasn’t booted up yet this morning, so I can’t remember the name of the model just yet, but my personal favorite is a fan source which couples blade element momentum theory into a momentum source to approximate the effect of real fans on your domain.

I’ll do some digging when I get to the office and give you a better answer.

I did try the Momentum Source before, not the fan option, which uses the unit N/m3 to define the source term, but the problem I had is that it was difficult to link a certain values of soure term to provide a specific value of thrust. For emample, 10% of calculated (target) momentum source can provide the target thrust which I need, while 100% of calculated momentum source was much more sufficient.

In my research, the fan is a simple geometry/module as I would only need it to be over the wing and provide certain value of thrust, then I can play around with the airfoil. I use a spreadsheet to calculate the fan intake and outlet parameters (velocity, Pt, Ps, Tt, Ts, diameters, etc.) from the known requirements: target thrust per fan, fan pressure ratio, and isentropic efficiency.

I do find an interesting thing with the mass flow optioned Pressure Outlet (fan intake as pressure outlet and fan exit as velocity inlet), when I scale up the previous geometry to full scale, which is about 5 times larger. The fan intake mass flow is correct now (58 kg/s which is the set value), and with smaller geometry the fan intake mass flow was limited to 39 kg/s regardless how high the target mass flow rate set. So I am wondering if the size of the geometry would limit the actual mass flow in 2D solution.

[fluid23]

Ok... I have had some coffee and my brain is working at normal capacity.

Generally speaking, you wouldn't want to have boundaries so close to your area(s) of interest. Boundaries can have a significantly unrealistic effect on the flow so it is best to keep them as far away as practical. Using an inlet/outlet arrangement as we have discussed could be inducing errors of which you aren't even aware. I have attached an image illustrating how I use this in modeling rotorcraft engine flows. In this model I was looking for inlet distortion so I made sure to put the mass flow outlet as far downstream as I could.

I was forgetting this was 2D, so my original thought of using the virtual disk model is inappropriate. You will not be able to use virtual disk or fan source methods as these are only available in 3D. However, you should be able to use the fan interface option, although, you will probably have to modify your geometry just a little. I think your general approach for using the momentum source would be valid.

As for the mass flow rates, those should have probably scaled down with your model. It is very possible that the inlet was choking at 39 kg/s if it was 1/5 the size of the actual geometry that would have taken in 58 kg/s.

I would suggest reading the help files on fan interface and see if it isn't a better solution for you.

[Tianyi]

Hello Matt,

Thanks again for your suggestions regarding useing the fan interface. After one week attempt, I finally failed to adopt this method. The fan interface did not accelerate the flow before and after the fan. I scaled up my geometry to actual dimension and shortened the distance between the fan intake and exit, but still left a very small width. To avoid the nacelle-wing coupling study, I had to attach the nacell on the aerofoil. Do you think the nacelle has to be completely off the aerofoil?

I believe my target is very simple: (1) identical intake and exit mass flow rate; (2) inlet velocity around 0.5-0.6 Mach (can be adjusted with different mass flow rate setting); (3) just choked nozzle (fan exit with Mach 1 condition), I am not sure if the fan interface can realise those. I did go through the starccm+ fan interface tutorial and has some ideas of my fan performance. To be honest, I dont know too much information for the fan I am using, as I am not doing the fan design. However, I can still calculate all the temperature, pressure, and velocity values for my fan settings. I believe there must be something wrong with my fan performance curve, which you can find the link below. I used the fan exit static pressure 26216 Pa minus intake total pressure 36760 to get a negative pressure change value, is it correct? And also, if I set the x-axis to mass flow rate method, does it constrain the fan intake and exit mass flow rate? Cuz I set the fan intake as target-mass-flow-rate optioned pressure outlet and fan exit as mass flow intake alongside with the fan interface witht the same amount of mass flow rate to ensure the identical mass flow rate, Or do I only need to use the fan interface and leave the fan intake and exit to be other boundary conditions as if I use momentum source the fan intake and exit can be set as walls? If you could offer any advice, it will be much appreciated.

My fan performance curve setting:
https://drive.google.com/file/d/1OrS...ew?usp=sharing

Best Regards,
T

[fluid23]

Regarding nacelle/airfoil collocation, from what I recall of your geometry that might be a good idea. The airfoil isn't really an airfoil in 2D if you have the nacelle stuck to a pylon attached to the airfoil.... sorry if I am not remembering things accurately. Ultimately, that needs to be your call based on what you are seeing and trying to accomplish.

I don't deal with fan curves very frequently, but I think you are off base. The curve should relate flow through the fan to pressure rise across the fan. Then you can define a system curve based on your losses (inlet/exit losses) and the intersection is your operating point. It cannot be arbitrary and I am fairly certain it shouldn't be the difference between inlet total pressure and exit static pressure. It sounds like I sent you down the rabbit hole with this, sorry.

Perhaps your best option are matching mass flow inlets with opposite sign and appropriate settings.

[Tianyi]

Hello Matt,

I think fan interface is a powerful tool, but I am running out of time. I will stick with the mass flow inlet settings and try to get some solutions. Much appreciated.

Regards