Hi there,

I am trying to simulate a flow past a rounded trailing edge, using CFX5 The inlet flow is at mach 0.8 and flows upon a flat plate, until it ends as a rounded trailing edge. A shock should occurs at the beginning of the rounded trailing, since the flow passage is increasing suddenly.

I have done this simulation with a k-e log-law model and it has converged but without any sufficient accuracy.

Therefore, respecting the y+ conditions, I have done the same simulation with a k-w and also a k-e 2layer model to get a better results. Meanwhile I cannot obtain a converged solution. I observed each time that near the shock the pressure start to oscillate (waves of pressure is then propagating) to end up with a fatal error.

Do you have any idea about the rightness of the k-w and k-e 2layer model when having a boundary layer/shock interaction ?

What could be done with the grid, to be more precise ?

...---...

Alex.

(1). You are dealing with a very tough transonic flow problem. (2). It is not just the turbulence model issue. the mesh, the solver, the b.c. etc..all can affect the convergence of the solution.

Thanks, I know, that it's not the easiest transonic problem.

Actually I'm doing this case with two geometries, a blunt TE and a rounded TE, from Inlet Mach=0.2 to Mach =1.2 and with the three turbulence models.

In two sentences : M=0.2-0.8 no problems. M>0.8 big problems with k-w and k-e 2layers.

Maybe just some tips for transonic B.C. could help me a lot. (I'm using OPENINGS at the top and the bottom of my domain).

Thanks

Alex

(1). I had run a transonic flow case once using CFX TASCflow. Most of the time, I used it for subsonic flow claculations. (2). If CFX5 is using similar aolution method, then the behavior is probably similar. (3). I had used Fluent/Rampant four years ago to run 2-D flow over a cascade airfoil at transonic flow with unstructured mesh. In that case, the trailing edge is round, and the other has trailing edge ejection. (4). It took two weeks to get the converged solution with extremely high local mesh refinement near trailing edge area. (to capture the trailing edge shock). The flow field probably was not correct, because I didn't have enough mesh point in the boundary layer. (5). My suggestion is: ask the vendor to show you the sample cases with shocks first, and ask for the proper treatment of the boundary conditions. (if the method can handle it) (6). My feeling is that a density-based method would be a better choice.

First of all I'll point out that your probably not running k-omega or the 2 layer k-epsilon model in CFX-5 as these models don't exist yet. What code are you actually using for those models?

If you were running CFX-5 with k-epsilon was it 5.4 or 5.4.1 or 5.3? Significant robustness and accuracy issues have been addresed in 5.4.1 with respect to previous releases.

Were you running with high resolution or fixed blend factor advection scheme?

I'd suggest that if your having these sort of difficulties you contact your service rep and get some help sorting it out.

Dan.

Sorry guys, I don't know why I wrote CFX5, I'm working on CFX-TASCFlow 2.10.0

Just a remark to your problems with the k-w and k-e 2 layers. Have you changed the grid such that you are in the valid y+ range at the boundary. Basically the same grid should not be used for a calculation with k-e and k-w. What kind of mesh do you use at the walls, I beleive (no proof) that you should not use a tetrahedal at the walls, better with inflated boundaries when using the k-w or 2layer. Jan

Hi, I have hands on experience with compressible flows using different splitting schemes and less with incompressible flows. I have done shock wave-boundary layer for a laminar case. But yours is a turbulence model. As had already been suggested by others,make sure (1)you're in the "right" y+ regime and your mesh refinement in the B.L (2)when it comes to shocks you better go for density based methods (3)you need to check the flow solver of the software in detail that is how does it treat cases involving reasonably strong/very strong shocks and the boundary conditions (through which physics enter the problem). If you tell more about it I can suggest someone who has done turbulence models using Roe scheme and some other splitting schemes. I don't have his email address

CFX-TASCflow uses a coupled implicit pressure based approach. You said that density based approaches are the way to go. Why?? I've used both, and as far as I can tell there's no fundamental reason that solving for pressure or density makes a difference if the discretisation is strongly conservative.

Numerically both have their own little quirks that you have to figure out in order to get them to behave well but either works just as well once you figure it out.

Dan.

(1). Well, just run a transonic cascade nozzle flow with a round trailing edge to find out whether you can capture the trailing edge shocks. Then tell us how well you are doing. (2). Flow through a cascade would be fine. That is the flow entering the cascade from left to right. Then make a sharp turn, exiting at, say 80 degrees. The Mach number aft the trailing edge should be around 1.2 And there should be a trailing edge shock coming from the round trailing edge. (3). Let us know how you solve the problem. Choice of the codes or methods is yours.

If you mean what I think you mean, I've seen flows like this calculated in gas/steam turbines in TASCflow before. The trailing edge shocks are captured just fine if you have enough grid. I'm not sure about the turning angle on the cases I've seen, but they were relatively high. CFX-5 would behave very similar. In fact it might even do a little better because it has a modern monotone advection scheme in it.

I've done 2D transient shock wave calculations in CFX-5, the same as those done in the early eighties by Paul Woodward and Phillip Collela (in one of their first papers on PPM in the Journal of Computational physics). CFX-5 does very well on these types of flows. It captures the shock waves to within a few grid cells and captures contact discontinuities within 4-6 grid cells. This is typical for most monotone advection schemes. Note that contact discontinuities are even harder than shocks, so I'm quite a bit more impressed when a code can do these well, because they do not numerically steepen like shocks as a result of acoustic wave characteristics converging along the shock's propagation path.

Dan

(1). I definitely would like to see the TASCflow shock capturing result for gas/steam turbine, if it's available on Internet(?). (2). I didn't say that it can't do, but I do like to see it.