Hi all,

I am trying to model the inlet to a swirl combustor. All I have from experiments is the swirl number of air, pressure of air entering and the mass flow rate.

Could anyone please advice me on how to specify such boundary conditions, especially, how do we specify swirl number?

Thanks Regards Sachin

Approximate approach :

1) Use velocity inlet.

2) Axial velocity = mass-flow-rate / (rho * Area)

3) Approximate swirl number = G_theta / Radius * G_axial

From 3), you can calculate swirl velocity.

For example, one veolcity inlet with axial and swirl velocity,

Swirl number ~= 0.6667 * V_swirl / V_axial

Most of all, you should search for the referencde about swirling flow.

Sincerely, Jinwook

Dear Lee,

Thanks for your reply.

I could use the above technique to calculate the maximum swirl velocity and then apply a solid body rotation to a pipe and generate the swirl and hopefully it should match the velocities.

But, I never did specify the pressure. I don't think we can specify pressure of air entering with velocity inlet.. do you suggest changing the operating conditions instead?

Thanks Regards Sachin

Of course you can not specify pressure of entering air.

But, it is needless to specify the pressure. Remember that all pressure is relative to the operating pressure.

Sincerely, Jinwook

Dear Mr. Lee,

I would say that this would be true as long as pressure has a linear dependance in the governing equations.

But, I guess pressure has a non-linear dependance and we may not be able to simply take relative difference. Could you please explain why pressure can be taken as a linear variable.

Thanks Regards Sachin

It seems that we can also use the pressure inlet boundary condition to model such conditions (pressure and swirl number)..

just specify gauge pressure and use "Direction Vector option" for Direction Specification method then Swirl number can directly be specified under the Tangential -Component of flow direction. The axial component will be Sqrt (1-SN^2).

What do you all think on this?

Regards

The axial component will be Sqrt (1-SN^2) ?

Then, how about when SN is larger than 1 ? Axial velocity is negative.

Sincerely, Jinwook

Is your problem high Mach number flow ? Otherwise, relative pressure determines the flow characteristics. And operating pressure is used to determine the desnity by using ideal-gas-law.

Sincerely, Jinwook

yes I think you are right.. but according to the manual the direction vector specification method expects us to specify the direction cosine.. it does not give us the magnitude of axial/tangential velocity, but, just gives us the direction where it has a tendency to move.. for example, specifying an axial direction vector of 1 would imply all the flow is in axial direction, while specifying the axial direction component as 0.5 would imply that the flow is partially towards the axial direction.. this percentage could be controlled by this direction vector specification method.

Now although the swirl number is different from direction cosines, but, give us an "approximate" figure on the direction cosine for the flow.. I don't know whether this approach is correct and am still trying to see its "correctness".

Ofcourse what you have specified seems to work out ok too, but, I was wondering if you expected me to specify a solid body rotation to the inlet flow or just the "swirl velocity" by the method you specified.

Thanks a lot Sachin

[azim8824]

i have make an experiment using a jet swirl hollow cone..did this formula can be apply to this type of atomizer..i have volume flowrate, pressure,angle of inlet, number of inlet..can anyone suggest how can i get a swirl number..really need help from all of u..

[juzer_700]

I have been trying to use ANSYS FLUENT Software to simulate cold flow analysis inside a combustion chamber. But I am having difficulties. It shows reverse flow when I run the calculation. My geometry is in 2D-Axisymmetrical. Also I have taken a swirl facter of 0.7 using K-Epsilon RNG turbulence method.

Inlet condition:
Velocity- 1m/s, Air at 600K
Pressure Outlet - Gauge pressure=0

Is the reverse flow because I have included the swirl in the flow? Or is it because my domain is small?

Do I have to mention swirl velocity also???? I have mention the swirl factor in RNG model.

I would really appreciate if you can help me figure out the problem. Thanks in advance.

[juzer_700]

Originally Posted by azim8824

i have make an experiment using a jet swirl hollow cone..did this formula can be apply to this type of atomizer..i have volume flowrate, pressure,angle of inlet, number of inlet..can anyone suggest how can i get a swirl number..really need help from all of u..

If you are using an annular swirler, you can calcluate Swirl number using this formula,

S= 2/3*(1-(ri/ro)^3)/(1-(ri/ro)^2))*tan(angle)

[azim8824]

Originally Posted by juzer_700

If you are using an annular swirler, you can calcluate Swirl number using this formula,

S= 2/3*(1-(ri/ro)^3)/(1-(ri/ro)^2))*tan(angle)

What is the meaning of annulur swirler..my atomizer is like a agriculture nozzle..i try to insert picture but it ask the link..hope u know the design inside the agriculture nozzle that will produce a swirl water..it is suitable for my atomizer?.hope all the readers can help me..

[Seroleh Osman]

To study more about swirl,
you can read my published paper at this link:
http://www.academicjournals.org/ijps...%20et%20al.pdf

[azim8824]

I had read your journal about radial swirler..i make a research about jet swirl atomizer but still in initial phase..may i know what is the meaning of contraction coefficient and air throat area..my jet swirl atomizer design is based on the common agriculture spray..i am still confuse to choose formula to get the swirl number..thank you for your journal..