Simulating high velocity airflow through a curved tube

[Anonymous]

Hi,

I'm trying to calculate the forces exerted on an air intake duct for an electric duct fan (EDF) . However, after running the simulation for many iterations, the velocity of the air and the forces exerted on the body keep getting rising with no end. I've tried the following setups with no luck:

1. Inlet velocity of 300km/h and unknown outlet
2. Inlet mass flow rate of 0.69 kg/s (equvilant of 300km/h for the tube) and an unknown outlet

Also, I tried using the compressible and incompressible flows and other suggestions from the Autodesk Sim CFD guides.

Tutorial: Internal Compressible Flow in a Nozzle

http://help.autodesk.com/view/SCDSE/2015/ENU/?guid=GUID-065F43DD-806B-4209-800F-8E61A0B23D9C

Internal Compressible Flow

http://help.autodesk.com/view/SCDSE/2015/ENU/?guid=GUID-D763685E-39F1-4CCE-B6C7-CDAC3217A5B2

What am I doing?

[Jon.Wilde]

Hi,

I would suggest you need a better inlet shape - can you extrude that face out normal to the surface with a length about 5x it's width? What direction does the flow actually enter, is it as shown here?

Same with the outlet - have a nice uniform cross section for a length about 10x the width if possible.

A few additional points:

• You need to ensure that your Total Temperature value is correct - this is under 'Solve -> Physics'
• Turn Auto Forced Convection off
• If this is compressible, we likely need to choose a different turbulence model, however:

Often with these types of analyses it is good for us to take a step back and check that we have taken the correct approach. What values do you know from real life? Flow rates/temperatures/pressures?

Are you certain that this is a compressible analysis? Isn't the velocity going to be 83m/s?

Thanks,

Jon

[Anonymous]

Hi Jon,

In this scenario the flow is not compressible - it would be at higher velocities. The things I know about the environment are that it's sea level conditions and a temprature of 20-25 C.

I took you advice and extruded the inlet and the outlet. The sim has become much more stable but I don't think the results are correct, because the flow goes -Z so I'd expected the Z Total Force to be negative but its showing a positive value. (Used ADV 1)

[Royce_adsk]

Can you attach your share file for us to checkout?

Thanks!

[Anonymous]

I made some modification and ran the simulation for over 10,000 iterations and this is the result. Attached is the sharefile.

[Jon.Wilde]

Hi,

Looking over some of your settings I see that you have mesh enhancement off and are running with the mixing length turbulence model. Is there a reason for these changes that I am not aware of?

I would tend to leave the turbulence model alone or use SST with an increased number of boundary layer elements.

ADV5 would be the best advection scheme to use here, expecially in conjunction with the SST turbulence model.

We should not need to apply surface materials to the external surfaces either, unless we are looking at wall roughness I cannot see a reason for this.

When you are taking the wall measurements, which walls are you selecting?

Kind regards,

Jon

[Anonymous]

Honestly, I was experimenting to see if I can get a stable output.

• I used ADV 4 because it's description sounded like its designed for such analyses (ADV 4 (Min-Mod scheme--Petrov-Galerkin variant)   •Moderate numerical stability (less than ADV 1)  •Specially tuned for flows in long narrow ducts)
• The measurment surfaces are all the middle ones. Basically everything, excluding the walls of the extended long ducts on both sides, the inlet, and the outlet.

Thank you for the continued help Jon 🙂 Let me try again and get back to you

[Jon.Wilde]

Super stable here with SST, I'd give it a shot.

I see the confusion with ADV4, imagine something like a hollow coil where the length is hufe vs the diameter, that is where we might use it. Here, ADV5 should be perfect.

Keep a close eye on your convergence too, ideally we want each variable to be very smooth.

This is not converged yet but looks OK to me, I think you may need to consider running compressible, as I am seeing some fairly negative pressure values in the narrowest section, just something to be aware of.