CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Main CFD Forum

High mach number flow

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   June 18, 2003, 02:39
Default High mach number flow
  #1
Logesh
Guest
 
Posts: n/a
I have a flow problem statement as follows,

There is a big cylinder connected to a small cylinder, which in turn connected to a big cylinder. That is small cylinder in between two big cylinders. One side of the cylinder is open to atmosphere and another side is connected to low pressure (Pressure is not known but less than atmospheric pressure, but velocity is known)

This is simulated in CFD by applying atmospheric pressure at the inlet condition and applying negative velocity at the outlet. Whether this boundary condition is appropriate?

The second issue at the small cylinder region, the velocity is substantially higher than sound velocity. It is in supersonic flow (Shock and sound waves are formed). What model to use in this regard?

Currently, I am using segregated solver+implicit formulation with standard k-E turbulence model with ideal gas relation for material property in order to account for the compressibility effects around the small cylinder region.

Whether coupled solver is preferred than segregated solver?

Looking forward for the suggestions/comments.

Logesh.E

  Reply With Quote

Old   June 18, 2003, 13:29
Default Re: High mach number flow
  #2
Jim Park
Guest
 
Posts: n/a
Are you talking about flow through these cylinders (an internal flow problem) or flow across the cylinders (an external flow problem)?
  Reply With Quote

Old   June 18, 2003, 22:55
Default Re: High mach number flow
  #3
logesh
Guest
 
Posts: n/a
It is an internal flow problem with maximum mach number of the order of 3.

Logesh
  Reply With Quote

Old   June 19, 2003, 07:27
Default Re: High mach number flow
  #4
logesh
Guest
 
Posts: n/a
hai,

In the manuals it is mentioned that coupled solver is preferred than segrgated solver high velocity compressibility flows.

I have to play with courant number in coupled solver in order to get convergence.

The other query, I have in this regard whether the mass flow rate wouldn't change beyond mach number>1.

I tried different boundary condition values(negative velocity) at the outlet, which resulted in, change in pressure drop.But the mass flow rate remained the same.Whether this is expected behaviour or something unusual?

Regards, Logesh
  Reply With Quote

Old   June 19, 2003, 11:36
Default geometry ???
  #5
Danny Tandra
Guest
 
Posts: n/a
I tried to understand the geometry of your problem here.

If the diameter of the cylinder is fixed (constant) then I don't think you can get supersonic velocity at the small cylinder.

For compressible flow in a pipe with constant cross section area: 1. if you start from subsonic flow, the maximum velocity that you can get is sonic velocity M=1 2. If you start from supersonic flow, the velocity will decrease to M=1.

D.Tandra
  Reply With Quote

Old   June 19, 2003, 13:31
Default Re: High mach number flow
  #6
Apurva
Guest
 
Posts: n/a
I guess you are using Fluent for this problem.

Best solution is go for Coupled solver with 2nd order discretization, use explicit solver, intially start with low CFL .., also do adaptation of grid on regular intervals based on Mach number i.e. around mach no 1. You will get better solution.

Regards

Apurva
  Reply With Quote

Old   June 20, 2003, 00:21
Default Re: High Mach flow geometry ???
  #7
logesh
Guest
 
Posts: n/a
Hai,

Tandra:- I explain the geometry once again.

The big cylinder is connected to inlet of small cylinder.The outlet of small cylinder is connected to big cylinder.It is similar to converging,diverging nozzle.The only difference is big cylinder aren't tapered.Therefore changes are stepped fashion from big cylinder to small cylinder diameter.

Apurva:- Thanks for your suggestions. I will try the same. Suggestions from fluent manual also in similar lines for high velocity compressible flows.

Have a nice weekend.

Logesh.E
  Reply With Quote

Old   June 20, 2003, 06:18
Default Re: High mach number flow
  #8
Nicola
Guest
 
Posts: n/a
As in a converging-diverging nozzle, mass flow rate gets its maximum value when back-pressure is lower enough to have a sonic region in the pipe. Once you have a sonic flow (if the flow were frictionless and adiabatic, this condition should be reached at the point of the minimum of the cross area) the mass flow rate doesn't increase even if you lower the back pressure. Of course, you will have a complex interaction of shocks and expansion waves after the sonic region. You can see by yourself that this shock system will change with the outlet pressure.

In my opinion, a velocity boundary condition at outlet plane is not the best choice because when Mach number goes to infinity then velocity reaches asymptotically its maximum value (k*R*Ttot)^0.5. I would use a pressure condition at outlet.

Hope it helps
  Reply With Quote

Old   June 20, 2003, 09:51
Default Re: High mach number flow
  #9
logesh
Guest
 
Posts: n/a
Hai,

Thanks for your valuable comments.

I will try to get pressure outlet condition.

"Once you have a sonic flow (if the flow were frictionless and adiabatic, this condition should be reached at the point of the minimum of the cross area) the mass flow rate doesn't increase even if you lower the back pressure".

Do you have any reference for the above statement.Some text book or web-site reference.I already searched in google,once again I will do it.
  Reply With Quote

Old   June 23, 2003, 02:03
Default Re: High mach number flow
  #10
logesh
Guest
 
Posts: n/a
Hai,

Whether increasing the small cylinder diameter will be of any help in achieving least pressure drop and the same mass flow rate.May be it is better to achieve mach number 1 or sligthly less than that in achieving maximum mass flow rate.

Regards, Logesh.E
  Reply With Quote

Old   June 30, 2003, 08:30
Default Re: High mach number flow
  #11
Nicola
Guest
 
Posts: n/a
Hodge, Koenig, Compressible Fluid Dynamics, Prentice Hall is the book I used during my studies, but I think you can look in many books concerning compressible flows.

I have found this link: http://www.engapplets.vt.edu/fluids/...le/cdinfo.html, I hope it will be useful.

Nicola

  Reply With Quote

Old   June 30, 2003, 09:03
Default Re: High mach number flow
  #12
Nicola
Guest
 
Posts: n/a
If you increase the small cilinder diameter then the mass flow rate at sonic condition will be higher. If your goal is the mass flow rate, raise the back pressure and increase the 'throat' area to avoid supersonic flow while keeping constant the mfr. If you want to have the same exit Mach number to study the shock interaction, then you have to use the same pressure ratio Pexit/Ptot_inlet: increasing the cross area of the small tube, while keeping the same pressure ratio, will reduce the shock intensity until the shock will disappear.

Nicola
  Reply With Quote

Old   June 30, 2003, 09:43
Default Re: High mach number flow
  #13
logesh
Guest
 
Posts: n/a
Hai Nicola,

Great and very useful reply.

The web-site mentioned is excellent and useful for my application.

Thanks for spending time in sharing your knowldege.

Regards, Logesh.E
  Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
pre-conditioning for low mach number compressible flow solver Shenren_CN Main CFD Forum 0 April 29, 2011 21:07
Low Mach number Compressible jet flow using LES ankgupta8um OpenFOAM Running, Solving & CFD 7 January 15, 2011 14:38
low velocity but high mach number? it is true! frank CFX 4 October 23, 2008 05:46
high mach number, and multiphase AdN FLUENT 0 April 13, 2006 09:40
Segregated vs Coupled, High Mach number flow? David Shkval FLUENT 2 April 14, 2002 07:30


All times are GMT -4. The time now is 05:37.