# High mach number flow

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 LinkBack Thread Tools Display Modes
 June 18, 2003, 02:39 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

 June 18, 2003, 13:29 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)?

 June 18, 2003, 22:55 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

 June 19, 2003, 07:27 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

 June 19, 2003, 11:36 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

 June 19, 2003, 13:31 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

 June 20, 2003, 00:21 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

 June 20, 2003, 06:18 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

 June 20, 2003, 09:51 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.

 June 23, 2003, 02:03 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

 June 30, 2003, 08:30 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

 June 30, 2003, 09:03 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

 June 30, 2003, 09:43 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

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Shenren_CN Main CFD Forum 0 April 29, 2011 21:07 ankgupta8um OpenFOAM Running, Solving & CFD 7 January 15, 2011 14:38 frank CFX 4 October 23, 2008 05:46 AdN FLUENT 0 April 13, 2006 09:40 David Shkval FLUENT 2 April 14, 2002 07:30

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

 Contact Us - CFD Online - Top