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?

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.

CFX-5 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 CFX-5 are you running?

Robin

CFX-5 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 CFX-5'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 over-refinement 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 1e-3 or 50 timesteps (whichever occurs first) and converge your solution to a MAX residual 1e-4 (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 CFX-5.

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.

Are you generating your mesh with CFX-Build? Which version of CFX-5 are you running and what IBM machine/OS?

Robin

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 CFX-5 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 CFX-5.

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.

(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 2-D 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 multi-shock 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 pressure-based 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. )

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.

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