
[Sponsors] 
June 28, 2001, 06:11 
Mach number Limitaions?

#1 
Guest
Posts: n/a

Is there a Mach number limitation using CFX 5. Inconsitencies in the solution to a two shock problem beyond Mach 2 when using CFX 5?


July 9, 2001, 04:34 
Re: Mach number Limitaions?

#2 
Guest
Posts: n/a

My experience is that CFX 5 cannot handle Mach numbers over 2 very well. It breaks down when the mach number is larger than 2.5.
It is still essentially a pressure based code. For highly compressible flows I recon it is better to use density based codes. 

July 9, 2001, 22:24 
Re: Mach number Limitaions?

#3 
Guest
Posts: n/a

CFX5 will continue to perform at Mach numbers well beyond 2. Can you be more specific than it breaks down? What type of problem are you running? Boundary conditions? Timestep? Rotating or stationary frame?
What version of CFX5 are you running? Robin 

July 9, 2001, 23:07 
Re: Mach number Limitaions?

#4 
Guest
Posts: n/a

CFX5 will solve your problem. You will have to ensure you are using the right boundary condition (ie. supersonic inlet(s) and outlet(s) where applicable) and start with a reasonable initial guess.
This is also where CFX5's automatic mesh refinement particularly shines. In fact, I would go so far as to say you should not run a supersonic case without adaptation, as you are not likely to know the exact location of your shock while setting up your initial grid (hence the CFD solution. Starting with a reasonable grid, you can let the solver refine as necessary around your shock, minimizing grid dependance and the tendency of for coarse grids to smear the shock. Before you use adaptiation, however, make sure you can get you problem up and running. Once you have figured out your b.c.'s and initial guess, you can write out a new .def file with the adaptation parameters set and use the previous grid (and solution) to get a head start. (The next time you run, use adaptation from the start, assuming you are confident about your setup). To adapt effectively around a shock: i) adapt by pressure and select the Variation * Edge Length option (this will prevent overrefinement about the shock); ii) adapt to geometry, in order to gain higher fidelity to the original geometry; iii) skew the adaptation to assign more nodes on the first step (value of 2 will suffice). Finally, you should trigger adaptation at a MAX residual level of around 1e3 or 50 timesteps (whichever occurs first) and converge your solution to a MAX residual 1e4 (or better). The remaining defaults will be fine. (You can also choose to save the mesh at each step. This is always useful to visualize the adaptation steps and quantify the added resolution. Intermediate meshes may also be used to estimate error.) Regards, Robin PS: You may also want to check out the CFX and search for Mach. This <a href=http://www.software.aeat.com/cfx/ilibrary/documents/dhinagaran_paper.pdf>paper is for TASCflow, but is equally applicable to CFX5. 

July 10, 2001, 02:56 
Re: Mach number Limitaions?

#5 
Guest
Posts: n/a

Unfortunately grid adaption does not work properly on a IBM machine. CFX does not retain the orgininal geometry. So starting with a coarse grid and then refining results in a poor geometry description in the finer grid.


July 10, 2001, 21:11 
Re: Mach number Limitaions?

#6 
Guest
Posts: n/a

Are you generating your mesh with CFXBuild? Which version of CFX5 are you running and what IBM machine/OS?
Robin 

July 10, 2001, 21:37 
Re: Mach number Limitaions?

#7 
Guest
Posts: n/a

CFX 5.4.1 is not able to adapt to geometry on the IBM platform. The version of fortran used to compile MSC Patran is an older version than used by the CFX5 developers. As soon as a newer compile of Patran is available, this issue will be resolved.
Geometry based adaption works on all other platforms supported by CFX5. 

July 10, 2001, 23:09 
Re: Mach number Limitaions?

#8 
Guest
Posts: n/a

What exactly is a two shock problem? You say it like we should all know what that is.
After we know what it is, then maybe you can describe the inconsistencies and your problems can be diagnosed. Dan. 

July 11, 2001, 04:25 
Re: Mach number Limitaions?

#9 
Guest
Posts: n/a

(1). I am not quite sure about his problem. (2). But, in most cases, the shock generated by a body or wedge will be oblique. When it hit the wall, there will be reflected shocks. (3). The smearing in the shock capturing scheme will be the major problem. (4). When you have two bodies or two wedges in the flow,say 2D inlets, there will be two oblique shocks generated, and these shock will intersect each other which will generate additional features of the flow field, such as the slip lines. (5). The other possible area is the multishock Mach disks in the supersonic jet or plume where the jet flow is confined withing two curved boundary shocks with reapeted Mach disks inside.(6). These problems require high accuracy scheme to capture the shocks and the shock induced flow field. It could be difficult for the pressurebased formulation to predict the flow accurately. (it is likely to be very diffused solution, I don't know. But it sure can be checked out easily by running some test cases. )


July 11, 2001, 23:31 
Re: Mach number Limitaions?

#10 
Guest
Posts: n/a

Yep, there are many situations where more than one shock is produced and they may (or not) interact to create various interesting flow features. I guess I was wondering which case this guy was referring to.
How diffusive the solution looks will depend on the grid and the advection scheme, not what primitive variables are being solved for. There is no evidence that a properly implemented pressure based solver should not be able to do a reasonable job on high speed flows. Even density based solvers can crash fatally when pressure ratios greater than 50 to 1 exist in the flow field. Dan. 

July 12, 2001, 02:47 
Re: Mach number Limitaions?

#11 
Guest
Posts: n/a

Grid generation > CFX build CFX 5 version 5.4.1 (latest patches) IBM rs/6000 44p 270 AIX 4.3.3.25


Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Mesh Refinement  Luiz Eduardo Bittencourt Sampaio (Sampaio)  OpenFOAM Mesh Utilities  41  January 17, 2013 03:43 
mach number and selection of the fluent solver  turbinesv  FLUENT  4  April 24, 2011 00:14 
Problem with decomposePar tool  vinz  OpenFOAM PreProcessing  18  January 26, 2011 03:17 
Strong oscillation at transonic mach number  martingariepy  FLUENT  2  May 12, 2009 11:40 
Trimmed cell and embedded refinement mesh conversion issues  michele  OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ...  2  July 15, 2005 04:15 