CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   FLUENT (https://www.cfd-online.com/Forums/fluent/)
-   -   Producing a supersonic flow in a constant diameter cylinder (https://www.cfd-online.com/Forums/fluent/102159-producing-supersonic-flow-constant-diameter-cylinder.html)

 clgs.1903 May 24, 2012 00:43

Producing a supersonic flow in a constant diameter cylinder

Hi,

I am trying to analyse the effect of a shock wave around a blunt body, by inducing a Mach 2 flow at the entry of a cylinder, which then flows past a sphere and then out the outlet. The cylinder has a constant diameter.

I had assumed I could produce this flow by altering the pressure boundary conditions, however I cannot get anything close to a Mach 2 flow to occur.

The fluid properties I defined were:
density = perfect gas relation
Cp = 1.6565 J/kg-K
Mwt = 17567.5 Kg/Kmol
viscosity = 0.5 Pa s

If my calculations are correct, this should result in a speed of sound of:
a = (kRT)^(1/2) = 50 m/s at T = 100 K.

I defined the inlet boundary condition as a pressure inlet with
Total pressure = 1951.252 Pa
Supersonic pressure = 249.37 Pa
which should give a density of 1 kg/m^3 at the inlet, from perfect gas law,
and thus an inlet velocity of 100 m/s.

I set the outlet boundary condition to a pressure outlet with P = 1000 Pa, as I am assuming a drop in pressure over the shock wave.

However, I end up with flow in the order of 1 m/s and no shock wave forming. I'm assuming that I've midunderstood how to use the boundary conditions, but this is the only way that it makes sense to me. If anyone has any ideas I would greatly appreciate it.

TL,DR - What boundary conditions should I set in a constant diameter cylinder to produce a supersonic flow around a blunt body within the cylinder?

 Far May 24, 2012 03:00

Quote:
 I defined the inlet boundary condition as a pressure inlet with Total pressure = 1951.252 Pa Supersonic pressure = 249.37 Pa which should give a density of 1 kg/m^3 at the inlet, from perfect gas law, and thus an inlet velocity of 100 m/s.
You should go for the pressure far field boundary.

Quote:
 I set the outlet boundary condition to a pressure outlet with P = 1000 Pa, as I am assuming a drop in pressure over the shock wave.
This should happen inside (local) the domain and should not propagate at outlet boundary. so at outlet you should define the 101325 and operating pressure zero.

Can you give details about the courant number, flow scheme , gradient option etc. Also post some pics of geometry, mesh and results obtained so far.

 clgs.1903 May 24, 2012 05:54

http://s18.postimage.org/5wbo0zj95/untitled.jpg

This is a picture of my mesh and geometry. The sphere is 1 metre in diameter, the cylinder 20 metres in diameter, and 45 metres long.

I'm using the density based solver, with the energy equation switched on. I've left the Courant number and other solver properties at their default values for now (I'm just trying to get an idea of how to get it to solve).

I tried implementing your suggestions. I set the inlet to be a far field pressure boundary with a Mach number of 2 and a supersonic pressure of 250 Pa. The outlet I set to be a pressure outlet of 0 Pa.

I wasn't sure what to set for initialization values, but I tried leaving the pressure and velocity as 0 and the temperature as 100 K (same as the inlet). However this caused the solver to complain about Temperature gradients being too large. Setting the initialization velocity to 100 m/s resulted in divergence. So... I don't really have any results at this stage!

Any more thoughts?

 Far May 24, 2012 06:12

make the outer wall as slip (specified shear with zero values). use the hybrid initialization and solution steering with very low courant number.

You are using inviscid solver?

http://www.cfd-online.com/Forums/mai...nvergence.html

https://www.sharcnet.ca/Software/Flu...ug/node840.htm

http://www.cfd-online.com/Forums/flu...nvergence.html

Not directly related but may be useful.
http://www.cfd-online.com/Forums/flu...sst-model.html

 Far May 24, 2012 06:22

I assume that the sphere is placed in the free stream. Correct me if it is wrong supposition.

 jwillie2000 May 24, 2012 08:01

How did you compute the speed of sound? Specifically, what value did you use for R? Your value for the speed of sound is too small given the values you have. Jimmy

 clgs.1903 May 24, 2012 10:45

Far,
I'm using the inviscid solver, and yes the sphere is in the free stream. I'll give your suggestions a go tomorrow, thanks :)

Jimmy,
You're completely right, I made an error in my calculations of the molecular weight. I went over them several times and missed my mistake every time. They should be:
• density = perfect gas relation
• Cp = 0.625 J/kg-K
• Mwt = 46561 Kg/Kmol
• k = 1.4
• R = 0.17857 J/kg-K
• a = (kRT)^(1/2) = 5 m/s at T = 100 K.
• Supersonic pressure at inlet = 17.857 Pa
• which should give a density of 1 kg/m^3 at the inlet
• and thus an inlet velocity of 10 m/s for Mach 2 flow
I'll try the new values out tomorrow, see if that makes a difference. Thank you so much! And sorry for making such a silly mistake.

 jwillie2000 May 24, 2012 10:58

May be i should have put my question this way the first time. It would be nice I know the material you are looking at? I seem to be missing this info. Is it air or what?

 clgs.1903 May 24, 2012 11:23

It's not any fluid in particular, I'm just tweaking the values to get the flow conditions I want, in terms of the Mach and Reynolds numbers.

 clgs.1903 May 24, 2012 12:04

I decided I didn't want to wait to try it, haha. I used the correct values, the pressure far field inlet, and the pressure outlet of 0 Pa. I set the Courant number to 0.1 and used Hybrid Initialisation with the "Use Specified Initial Pressure on Intlets" command selected. And...

Success!!!

http://s14.postimage.org/ds3anuu0x/flow.png

This image is of the velocity vectors coloured by Mach number, in a plane parallel to the flow. The majority of the flow is at Mach 2 with just a small area around the sphere affected.

Thank you both so much for your help, hopefully I can progress a lot faster now that this problem has been figured out :)

 Far May 24, 2012 12:17

are you interested in boundary layer as well? what about vortex shedding? What's the Reynolds number.

These question are just for my knowledge and not related to your queries.

could you please post the Mach no. contour plot?

 Far May 24, 2012 12:19

Flow is steady state or transient?

 clgs.1903 May 24, 2012 13:41

The flow is transient, and I'm not interested in boundary flow or vortex shedding at this point. It's more of a test to see what can be done. Not sure on the Reynolds number, looks to be about 30000, but I'm not sure. I'll upload the contour plot when I get a chance :)

 All times are GMT -4. The time now is 19:40.