To anyone who may be able to help in this subject:

I have been working on the CFD simulation of an axial fan now for a few months. None of my results have been close to that of the empirical data tested on the particular fan.

Even such relationships as the speed of the propeller versus volumetric flow does not hold true, and in fact as the speed increases, the outlet flow decreases!!

With boundary conditions as inlet and outlet pressure conditions, and speed of the prop(rotor), I was hoping to solve for outlet mass/volume flow. This seems less and less likely as simple relationships cannot even be followed.

Lastly, the way a fan works is that IT creates the pressure, whereby outlet pressure will be higher than inlet pressure. CFX does not allow the fluid to flow against this adverse pressure gradient even with the prop rotating at 11,000+ RPM.

ANY HELP? IDEAS?

Thanks to anyone who can advise!!

-Giovan

Setting inlet and outlet pressure as boundary condition will let the simulation go freely to hit the target flow rate, which is more difficult than pressure on one end and mass flow rate the other end.

I do not think this is true: CFX does not allow the fluid to flow against this adverse pressure gradient even with the prop rotating at 11,000+ RPM.

Thanks Bian. I understand that setting pressures on the outlet and inlet is more difficult to achieve convergence, but from a design point of view, all I initially have is a pressure differential of which the fan needs to produce some flow against.

As I set the steady state simulation to have zero pressure differential (inlet = outlet), CFX generates ZERO mass flow. This is just not realistic.

I know you have worked on fans yourself, have you ever had any problems alike to mine?

If you are getting zero mass flow, you probably have the inlet or outlet (or both) totally walled off. Check that your rotational direction is correct. If the sign is wrong, the rotor would force the flow from outlet to inlet, causing a wall off resulting in zero mass flow.

Are you using steady rotor-stator MFR? If inlet and outlet have same pressure, theratically zero mass flow is the solution. Any flow would result in pressure difference.

I would suggest you setting total pressure (most likely zero) at inlet and mass flow rate at outlet. Then check the solution is correct or not, and how much static pressure difference between inlet and outlet. These can check if your case is right and give you rough idea the relation between mass flow and pressure difference.

One more thing: for the fan simulation, in most time it is not only one point simulation, it is several points on the flow rate vs pressure (BHP or efficiency) curve. Therefore, there is no need to set pressure at outlet, set several mass flow rates to get the curve.

I guess the problem I am having is trying to model this fan and match up its aerodynamic performance with the performance of which is tested empirically.

When a fan is said to be at a free flow state (alone in a room with no back pressure) in testing via AMCA standards, there is zero pressure differential from inlet to outlet. This is where the flow is maximum. I understand that theoretically there should be zero flow without any pressure drop, so maybe you are correct in the fact that I should not be putting a static pressure condition on the outlet.

I will try this and see what results I get. Again the hardest thing for me is trying to reverse engineer this fan using CFD, but not use the general principles of fan engineering (which is based on these standard empirical test procedures) which I have been accustomed to using.

Thanks to both of you for your help and concern.

wat are you boundary condition , can u past image of your mesh file???

My boundary conditions that I would like would be pressures on inlet and outlet. The MAJOR problem with this software is that even with the propeller rotating at 11,000 rpm (which causes an increase in static pressure downstream) the flow will not propagate against an adverse pressure gradient.

The inlet should be ambient pressure or close to zero gauge pressure, and the outlet pressure is higher and depends on whatever impedence the fan may be facing at the time. Then from these conditions the single most important variable to find is mass or volumetric flow.

I cannot post a view of my mesh file but would be willing to email it.

Free air delivery for a fan is "That point of operation where a fan or an air curtain unit operates against ZERO STATIC PRESSURE". Who says it is zero pressure differential?

You're right its not zero static differential. Free flow is when there is no impedance on the exit of the fan (imagine a fan in the middle of a room). This does not mean that internally there is zero pressure differential. Internally there must be a pressure increase downstream, even in "free flow" state. This is the issue with the program.

Has anyone ran fan models in transient state? I have had difficultly becuase of the problem with start-up and ramping up the rotational speed.

Hi,

I have worked on Compressors. I think this may help you.

In compressors, i used to give Total pressure at inlet & Static Pressure at Exit.

In fans, there is conversion of static head into Dynamic head.I think you adopt this principle also for setting Boundary conditions.

Regards aero

Giovan,

Are you applying static or total pressure at your inlet?

-Robin

Hi Giovan,

It sounds almost certainly like you have specified static pressure at your inlet, rather than total pressure. This would lead to the behavior you are experiencing. The static pressure in the room may be at atmosphere, but the dynamic pressure is nearly zero and therefore the total pressure is equal to your static pressure. This is not the case at the inlet of your fan. At the inlet, the static pressure will decrease as the mass flow rate increases, with the total pressure remaining nearly constant.

At the outlet, if the fan dumps into the room or plenum through a sudden expansion (i.e. there is no diffuser), the dynamic pressure will not be recovered and a good approximation is that the outlet static pressure is equal to the room or plenum pressure.

In the relative frame you will always observe a drop in static pressure, but the stationary frame total pressure will rise.

Run your fan curve again with Ptotal_in = Pstatic_out and you should see the behavior you expect.

Regards, Robin

Thank you Robin, I will try again. I have been running the simulation with the total pressure at the inlet along with either static pressure outlet or mass flow outlet and have not had much success doing so.

When you run a simulation do you run steady state or transient? I have tried both, and when running either I am not sure how to set my timestep to account for the high rotation of 11,500 RPM.

Thanks for the responses.

Giovan

Hi Giovan,

Run it steady state. The auto-timestep will be .2/omega, where omega is the rotation rate in radians per second. This should work relatively well, although you may be able to accelerate convergence by specifying a physical timescale of 1/omega.

-Robin

[genigood]

Originally Posted by Giovan
;79976

Thank you Robin, I will try again. I have been running the simulation with the total pressure at the inlet along with either static pressure outlet or mass flow outlet and have not had much success doing so.

When you run a simulation do you run steady state or transient? I have tried both, and when running either I am not sure how to set my timestep to account for the high rotation of 11,500 RPM.

Thanks for the responses.

Giovan

Hi Giovan,

I would like to know if you've been solved your problem ? because I have the same problem during a simulation of an axial fan, I get huge values of outlet pressure.

Please, answer me on my email : abdourabih4@hotmail.com

Thanks !

[Gkchpa]

Originally Posted by Giovan
;79976

Thank you Robin, I will try again. I have been running the simulation with the total pressure at the inlet along with either static pressure outlet or mass flow outlet and have not had much success doing so.

When you run a simulation do you run steady state or transient? I have tried both, and when running either I am not sure how to set my timestep to account for the high rotation of 11,500 RPM.

Thanks for the responses.

Giovan

Hello Giovan , I hope you solved above posted Issue, I am running similar simulation , and checked pressure boundary conditions and my results are far away from the real world results , so can you let me know how did you fixed it ? have you changed any boundary conditions ?

Thank You

[karachun]

Giovan is retired many years ago, his last post is dated 2007.