# High Mach number flows

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

 May 2, 2005, 21:57 High Mach number flows #1 Riaan Guest   Posts: n/a Hi guys, I am looking at a axisymmetric cone at high mach numbers (M=4.0 to M=10). The geometry is realitively simple, but I would like to know if FLUENT can model the physics. Right now we are using Newtonian impact theory to get a first-order feel for forces....but would like some CFD to back it up. Thanks ! Riaan

 May 2, 2005, 22:41 Re: High Mach number flows #2 Rajesh G Guest   Posts: n/a Ofcourse Fluent can catch the flow physics very well! I am also doing almost the same problem. ..and it can give the force data as well

 May 2, 2005, 22:48 Re: High Mach number flows #3 Riaan Guest   Posts: n/a My problem is that my experience is limited to supersonic flow at best - what is particular about hypersonic flow - currently we are using Newtonian impact theory, and I know that first order estimate.

 May 2, 2005, 22:52 Re: High Mach number flows #4 Rajesh G Guest   Posts: n/a I too am not used to hypersonic flows. Still, I have seen good results for hypersonic flows using fluent. Please refer to the following paper JFM 1997, Vol.352, pp 1-25

 May 2, 2005, 23:17 Re: High Mach number flows #5 Harish Guest   Posts: n/a I have had problems of fluent diffusing the shock for laser ablations in supersonic flows around mach of 3 .

 May 3, 2005, 03:43 Re: High Mach number flows #6 Razvan MAHU Guest   Posts: n/a Hi Riaan, I recently studied a M=3 and M=5 flow over a bullet with hemispherical head and obviously, with a very strong and detached hyperbolc shock wave being generated by this shape. I must say that the results were increddibly good taking into account that Fluent is after all a general purpose code. The secrets for accuracy and stability are: - use a structured grid ALIGNED WITH THE SHOCK (this is done by first calculating the deflection angle and then splitting the flow domain whit a line with exactly that angle, starting from the nose, of course, and then construct the grid) - stretch the grid cells very much close to the shock, just like you do with a boundary layer (definition of the shock depends highly on this) - use ONLY first order discretisation for all the variables, including flow, and COUPLED IMPLICIT solver with medium CFL (no more than 2-3) - if you want little more stability, use turbulent calculation starting from a inviscid one, with y+ around 1 - DO NOT make a sharp cone, round it off a little, it will not affect your results and will give you extra stability (you will also be able to make a structured grid this way) - use a small extent of the flow domain in front of the cone, not more then 2-3 times the cone's diameter (it is absolutely no reason to use more, the flow is completely supersonic, no information goes in front of the shock) - DO NOT adapt the grid, if you see that you didn't quite made an alligned grid, it is better to make a new revised grid. Do not be worried about the high number of cells you will have to use, but belive me, it would not compare with an unstructured adapted grid. If anything above seems hard to make, trust me your effort will not be in vane, there is no other BETTER way to do it. Best wishes, Razvan MAHU

 May 3, 2005, 03:57 Re: High Mach number flows #7 Luca Guest   Posts: n/a Thanks Razvan for your suggestions. I was looking for suggestiongs for supersonic, hypersonic flow modeling. Only a question: why do you use the 1st order discretization? just because your grid is so fine that 1st order gives results equal to 2nd order? Luca

 May 3, 2005, 11:56 Re: High Mach number flows #8 Razvan MAHU Guest   Posts: n/a That might be a good reason, to say so, but not quite... You see, making a "boundary-layer" type grid around the shock wave will never give you a flow aligned with the grid, so 2nd order discretization is a MUST for obtaining high quality results. But, in this particular case, 2nd order simply doesn't work (most cases computation diverges or you can't obtain a converged solution). On the other hand, we're talking about supersonic flows and with such high velocity, the fluid passing an oblique shock will not enter subsonic domain, so the flow has a well defined dominant direction, which in case of highly streched grid cells around the shock, will have distinct, opposite cell faces to cross, so 1st order will provide enough accuracy (to give an answer to your qestion). Also 1st order discretization is a more diffusive scheme than 2nd order, so the computation will surely be more stable. But be carefull, you should always start a comutation using 2nd order and EVERYTIME after obtaining a converged solution, you MUST try a 2nd order, even a QUICK solution. In my case, the bullet was very small (10 mm in diameter)and this could be a reason for not obtaining a stable 2nd order solution (at least for lower velocity), but I am pretty sure that for hypersonic flows only 1st order works. Best wishes, Razvan MAHU

 May 4, 2005, 11:29 Re: High Mach number flows #9 Luca Guest   Posts: n/a Thank you so much for your answer.Luca

 May 7, 2005, 15:49 Re: High Mach number flows #10 Roberto Guest   Posts: n/a Hi, does anyone know if fluent can be used for hypersonic flow that occurs when a vehicle re-enters the atmophere (Mach -> 25, chemical dissociation and reactions)? Thank You Roberto

 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 Roland R CFX 3 May 11, 2010 18:27 chelvistero OpenFOAM 11 January 15, 2010 20:43 Andreas CFX 1 March 13, 2009 06:58 frank CFX 4 October 23, 2008 05:46 Oliver Gloth (Gloth) OpenFOAM Running, Solving & CFD 0 December 20, 2004 08:30

All times are GMT -4. The time now is 07:46.