Validating Jet fan Simulation

[fattywin]

Hi,

i am trying to simulate a jet fan throw but i cant seem to get an incompressible steady state fan throw result.

This is how my jet fan looks like. the outer shell (232mm dia, 748mm long) serves as an outer casing of the fan itself. the disc located inside the casing (140mm dia, 20mm thick) serves as the rotating blade. all boundary conditions of the fan are set on the disc (rpm, vol. flow rate).

Jet fan condition

RPM: 2950

Flow rate: 630 CMH

And is it possible to assign gravity into this simulation ? does gravity affect the end results ?

I have the file below.

hope to get some helpful inputs.

Thanks,

Edwin

[Jon.Wilde]

Hi. I have a few points that should help you here:

1. We cannot set internal Boundary Conditions, remove these
2. Consider using the Axial Fan material to drive the flow
3. Using the fan material - it might be wise to have it touching the sides of the cylinder rather than having a leakage path
4. The mesh looks like it needs to be finer - the fan material will need a uniform mesh with 4-5 elements from the inlet face to the outlet
5. We cannot open a CFDST file and would need a CFZ

Thanks,

Jon

[fattywin]

Hi Jon,

Here is the cfz file and in the meantime, I will look into the few points that you have pointed out.

Thanks,

Edwin

[Jon.Wilde]

I think if you follow the comments you should be OK.

Is there any reason why you have a square jet fan inside a cylindrical tube though? I suggest you just make it fit the tube and also make it about 5-10x the length so that you can have a nice uniform mesh on it with at least 5-6 elements from inlet to outlet.

Thanks,

Jon

[fattywin]

Hi Jon,

Thanks for the reply. I've done what you told me to but I still can't get the throw(36m +-10% at 0.25m/s) I want.

Material

Fluid: Air

Solid: Aluminum

Internal Fan: flow speed = 630CMH, RPM=0.

I've attached my file below. Please help me check where have I gone wrong.

Thanks,

Edwin

[Jon.Wilde]

A couple more points after looking at your model:

1. Do you think that the very low flowrate on the inlet behind the fan might be restricting the amount of available air? Why not use a P=0 and leave it open?
2. You have only run for 200 iterations and the solution is not converged - a quick way to check this is that all the lines in the convergence monitor are flat
3. Under Solution Control -> Advanced, change the Convergence Assessment to 'Tight' so that it does not converge early and run for at least 1000 iterations - does it look converged then?

Kind regards,

Jon

[nhahn]

Agree with the above. Especially the inlet BC seems odd -- unless you have a reason for that it will cause the flow to recirculate instead of flow from inlet to outlet.

In addition to those suggestions,

1. you may wish to switch to advection scheme ADV 5.  The default advection scheme tends to have excessive dissipation (the price for stability).

2. the mesh you have is too coarse in the extended jet region to resolve it well, which will also lead to artificially fast dissipation.  Two options: put a cylindrical refinement region around the axis of the jet (say 2-3x fan tube diameter), and/or once it's running, turn on mesh adaptation (especially free shear layers) it should help reslove the jet better.  Uniform meshing can be turned off, and allow coarsening, then it will speed things back up a bit.

[fattywin]

Hi Jon,

Sorry for not replying after so long, have been trying out various way to do it but still can't get the result I want.

I did the amendment that I've been told here is the picture of the result: 

It did have a nice profile but I still can't get the throw distance I want which is 38m @ 0.25m/s.

Below is the file.

Thanks,

Edwin

[Jon.Wilde]

Hi,

Just looking at your image I would suggest two things:

1. It looks as though your outlet could do with being longer - we are clipping the results a little I believe
2. Your model does not look converged - the plot is still changing with each iteration. Can you tighten the convergence criteria and run for longer, or turn the convergence assessment off entirely? (Solve -> Solution Control -> Advanced)

Kind regards,

Jon

[Royce_adsk]

Keep in mind since you have no RPM to this fan you are limiting the peak velocities to the average velocity. This would probably reduce the throw.  A not so often used feature of the internal fan is the ability to assign a velocity curve at the outlet.  http://help.autodesk.com/view/SCDSE/2015/ENU/?guid=GUID-3672359B-4F6A-43FF-9308-5E9562ADB4CB

Where does the throw distance target come from?  Does it come from other simulation, testing, hand calculations?

What is the current distance of the throw in your simulation ... how off are you?

We should probably be doing this simulation in a 2D analysis so that we can improve runtime.

Best regards,

[fattywin]

Here is the pdf file of the fan I want to validate (PFS-30L with air flow 10.5CMM)

[Jon.Wilde]

Hi,

Don't forget that you do need a shroud around the fan - best to use a solid although I am using a surface material as I do not have the CAD.

Place a monitor point at 38m from the fan (right click during the setup to add one, you can track this during the run in the convergence plot, which will be hugey useful here).

What velocity value are you seeing at this point exactly, just wondering how far from the predicted value you are.

Thanks,

Jon

[rnkm.12]

Hi, I'm replying for fattywin. The definition of the maximum throw is the distance of that 0.25m/s contour line from the fan. We are always getting between 60m - 70m. We have also been using internal fan and centrifugal blower material, with and without shroud, with and without RPM. We just could not get the throw at 38m. Regards, Raymond