Dear all,

I have a relatively simple problem to solve: a transonic flow over a 3D wing. Obviously, there are some strong shockwaves on the upper side of the wing, and I have experimental data for their location (Cp distributions).

I am an experienced Fluent user, and I have computed this particular case as a verification benchmark with every Fluent version since 6.1. I never had any serious trouble, probably because of my experience too. And the results were almost excellent everytime: perfect shock strenght, and very good shock position prediction.

Now I'm trying to do the same with CFX 11, for the first time. I used the same mesh as for the last Fluent computation, a 2 million elements, fully structured multiblock mesh, of exceptionally good quality (smoothness and orthogonality). The CFX model settings are similar to those in Fluent, nothing new here. Everything seems OK, but the results are rather disappointing: shock location is acceptable, but the shocks are way too smooth! For this computation I used the High Resolution discretisation scheme, with Automatic physical time, SST-kw model.

Realizing that CFX is probably switching from 2nd order to 1st order near the shockwaves, I tried to use a 0.75 blending factor, as recommended by the user help, and impose the physical time by hand, decreasing the automatically calculated value about 20 times (from 2e-02 to 1e-03). Computation diverges after 10 iterations or so, with an absurd value for Mach number (in the order of hundreds). I tried to lower the physical time even more, to 1e-04 (that's 200 times smaller than the automatically computed conservartive value!!), but it only diverges later!

I probably cannot lower the blending factor any more because I will make the solution too diffuse and get the same smeared shocks, and a lower physical time is not a great option, I don't want to make 1000's of iterations to get a converged solution.

Could please anyone give me a hint? Or at least explain to me this unstable behavior of CFX? Because I cannot belive that for a relatively simple transonic flow, CFX cannot offer a 2nd order accurate solution!?

One info that might help: the region where Mach numbers are skyrocketing is somewhere near the leading edge, close to the symmetry boundary. And by the way, the converged High Resolution computation results were used as initial condition for the other (failed) computations.

All the best,

Razvan

Have you set the "max continuity loops" to 2?

It may be the cause of your stability problems for high-speed flows.

You will find the setting (in PRE) under:

Insert->Solver->expert parameter->convergence control->high speed models->max continuity loops

Hello Brendan,

Unfortunately I do not own such advanced knowledge of CFX to be able to figure out a solution like the one you suggested.

I will definitely try that, but is it too much to ask if I wanted to know what exactly should be the effect of this parameter, or what judgement led you to this conclusion?

Thanks a lot,

Razvan

Max continuity loops to 2 is a good option. Keep running on high res as you should swith automatically to first order around the shock wave (kind of upwind splitting function). I'm surprised you cannot get a sharp shock. I have read something about the "Carbuncle fix control" expert parameter, but this should only be applied when you cannot get a converging/stable solution.

Bart

Having 2 continuity loops means the solver has a 2nd pass (within each iteration) at the density*velocity relationship within the cells.

Oh, so it's something like "residual smoothing", which is a common stabilization technique for coupled solvers (Fluent has it for the coupled explicit solver).

Thank you,

Razvan

The "Carbuncle fix" is just adding some artificial dissipation to the shock-wave region, thus smearing the shocks even more. The problems seem to come from the LE area, not the shocks.

Razvan

But isn't there a flux or slope limiter implemented in CFX to take care of the numerical oscillations of the high order scheme near a shock-wave? This way it wouldn't need to switch to a low order scheme to maintain stability...

Razvan

You're right. In order to get sharp shocks you need to swith from second to first order. This is done automatically in the high res schema of CFX. Are you sure you have adequate grid resolution near your shock? 2 million cells sound a lot but it is 3D. Normally it should not be a problem specifically with a hex mesh (which should give the best resuts). Can you show a cross section picture with Mach number around the shock with the grid as overlay?

Hi,

Was the Fluent simulations done using the density based solver or pressure based solver? CFX does not have an equivalent of Fluent's density based solver.

Regards, Glenn Horrocks

Hello Glenn,

You have a point there, it is true that the density-based coupled solvers from Fluent compute slightly sharper shocks than the pressure-based coupled one, but the difference is not necessarily generated by the base-variable! The pressure-based coupled sover is NOT really a coupled solver, it only couples pressure and momentum equations, density, temperature and of course turbulence equations are still solved in a segregated manner. In my opinion, this is the main reason for its shock diffusivity.

And yes, I have used both density-based and pressure-based Fluent solvers, but the difference is too small to bother, and they both give much sharper and better placed shocks than CFX.

Interestingly, the 1st order solution from Fluent compares very well to the 1st order solution from CFX. But while the 2nd order solution from Fluent is really a 2nd order one, CFX's High Res solution is a mixed result, and that must be the only reason for the big contrast.

I'd like you all to understand that obtaining a good 2nd order solution for such a flow problem in Fluent is not a walk in the park, it does take some degree of skill, and I thought it must be the case with CFX too, that's why I asked for help on this forum. And I'm sure that there must be a solution, I just cannot see it yet.

All the best,

Razvan

Hello Bart,

I could of course show you that picture, but it is useless. The exact same mesh has been used for both solvers, specifically for having a fair comparison! And believe me that it is sufficiently dense both on the wing surface and normal to it for a decent Cp distribution.

Razvan

It looks like you're stuck. Ready to talk to Ansys?

Bart

Part of your problem is I don't think you are comparing apples to apples.

The DBNS solver in FLUENT uses Roe flux difference splitting. So, it will get a sharper shock than CFX or the FLUENT pressure based solver. Shock "sharpness" has nothing to do with coupling and everything to do with how the advection and pressure gradient terms are discrtetized so you might want to reconsider your opinion.

If you want to apply similar discretisation schemes in CFX & FLUENT then you must run FLUENT with the coupled pressure based solver and the second order upwind scheme. Both codes implement variants of the Barth & Jesperson limiter. That is the only apples to apples comparison.

Dear HekLer,

You seem to have read between the lines my response to Glenn:

"And yes, I have used both density-based and pressure-based Fluent solvers, but the difference is too small to bother, and they both give much sharper and better placed shocks than CFX."

For all tests with Fluent, the 2nd order discretization scheme was used for pressure, momentum, density and temperature, and 1st order for turbulence quantities.

I have already compared apples-to-apples. Almost...

I think I need to clear something out: the purpose of this computation was by all means NOT a comparison between CFX and Fluent, but a self-training in the future use of CFX. And I allways use an experimentally documented case in such situation, to get the necessary confidence. The fact that I involved Fluent in this dialogue, was just for you to understand that "I've been there, I've done that" already, I'm not a rookie at the beginning of his CFD journey. My final goal is to understand and be able to use CFX at least just as well as I've been using Fluent for the past years.

When the things went bad with this attempt to compute an old case using CFX, I wasn't blaming the software, I was blaming MYSELF. Because I know very well what kind of mistakes one can make the first time of laying one's hands on a new toy. So I turned to this forum, thinking that it must be the best way to find the solution.

And I still believe that there is a solution, because I find it hard to accept that I cannot get CFX to run a true 2nd order solution on this damned wing! When that will happen, I am convinced that the difference between the two codes will vanish.

Please excuse this long justification, but I felt it was needed...

All the best,

Razvan

Hello Brendan,

I have just tried that, but to no succes. I've even tried to under-relax the solution using the expert parameters, but again, with no positive outcome.

Thank you anyway,

Razvan

OK, sorry, did not mean to nitpick because you have to be careful.

If you have run the same hexahedral in both codes using:

- FLUENT coupled or segregated pressure based solver with second order upwind differencing. - CFX with High Resolution. - Got well converged answers in both codes (imbalances are good, residuals are low, etc...) with all three solution methods

and still get different answers.

Then there is either a setup error or there is a bug in CFX but I don't know what.

Check turbulence quantities, check boundary conditions are identical, check check ....

Dan

BTW, this is also a bit of a loaded statement:

"The pressure-based coupled sover is NOT really a coupled solver, it only couples pressure and momentum equations, density, temperature and of course turbulence equations are still solved in a segregated manner."

The fact that certain equations are coupled and others are not is not really the point. The point is if the code is implicitly making the important couplings. Implicitly coupling energy and turublence in with the hydrodynamics equations gets little benefit for a increased cost in memory footprint as well as assembly time. More important is the continuity and momentum coupling. Energy is not that important.

Dan

Well, it depends on the flow regime, or the physics involved, or both, doesn't it? If there is a strong physical coupling between all variables, then it would be beneficial to add energy and density to the list... For example, I cannot see how one would compute a supersonic / hypersonic reacting flow trouble-free, without using a fully coupled equation system.

That's why this partially coupled pressure-based solver of Fluent is not recommendable for very high velocity flows (I believe that's in the help too).

Razvan

CFX can be used for this kind of flow and I'm sure the CPBS in FLUENT could also handle it fine. The help just steers you to the DBNS solver probably because FLUENT has more experience with this type of flow in the DBNS solver.