hi every body

i use fluent to slove supersonic invicid flow about 2D cylinder, at postporceccing stage i saw at rear part there is recirculating flow; i can't imagine the source of this recirculating flow. any one help me. best regrads.

I used few times fluent for 2d inviscid cases. I saw the same, for example, with the flat plate at leading edge.

I think, but i'm not sure, that this is due to the numerical dissipation introduced by the scheme.

This happen where you have strong gradients and a poor grid quality (leading edge of a flat plate or rear part of a bluff body).

Try to improve the mesh quality in the separation zone or, if it's possible, increments the order of the scheme. Remember to take the cells size more uniform as you can too because this improve the mesh quality also.

may be it is the von karman street.

Dear Ali,

Karman street appears when the flow is viscous...

Did you set the boundary conditions to no-slip by accident??

Another thing - do you see shock waves at the back of the cylinder? Just a wild guess, but maybe the grid doesn't capture those and a further expansion is not possible, because you would reach negative pressure ...

Right. could you please send a pressure conture graph to my email. i am very peery of it. ali.

Check out my answer to a very similar question posted recently:

http://www.cfd-online.com/Forum/main.cgi?read=51584

I am actually wondering how you guys can expect such solutions to work out (inviscid flow over blunt bodies and flat plates).

I wonder where guys like you learned your CFD skills and knowledge!

>I wonder where guys like you learned your CFD skills and knowledge!

At university and at work, mostly through research.

The reason why I am questioning the approach is this: Although potential solutions as well as viscous solutions exist for these flows, Euler flow (inviscid, rotational) is somewhat problematic and not simply an intermediate between potential (irrotational) and viscous flow. Just take the flat plate at non-zero angle-of-attack as an example. Viscous flow will simply separate from the leading edge, and that's the only "real" solution. In inviscid flow, the sharp leading edge provides a singularity for velocity. That's not a big problem for potential flow (you can even construct an analytical solution), but a clean numerical Euler solution won't exist because of numerical dissipation. This numerical dissipation locally acts similarly to real dissipation (a viscous effect) and your Euler flow will tend to separate. Because inviscid separation is completely dependent on numerical dissipation, this solution will neither be "real" nor accurate. Likewise, the separation and re-circulation region behind the cylinder is a phenomenon that is real in the viscous case, but is a numerical artifact in the Euler case. Certainly, you could try to minimize the effect of numerical dissipation, but maybe you should just ask yourself if what you're doing really makes sense. Why not run a viscous computation?

two things:

Inviscid subsonic or incompressible flow around a cylinder is normally used to check how much numerical viscosity you have in your scheme. I don't think that anybody actually tries to get any real world problems solved by this type of computation. Any solver that produces a recirculation for this case with an Euler wall as boundary condition can be considered wrong I dare say.

The case in question is supersonic and that is a hell of a different story. For supersonic flow an inviscid computation can separate and it has a physical background. Consider a flow around (or better said along) a rocket shape at lets say Ma=5. At the base (the bottom of the rocket) you will get a separation because the flow is not able to expand around that corner (Prandtl Meyer expansion). If it would it would reach negative pressures. What will happen is that the flow expands and turns (and hence accelerates) as much as possible which is less than 90 degrees. Towards the symmetry axis you will get an oblique shock to re-adjust the flow to be parallel. This pattern can be re-produced by an inviscid solver. Now, what will also happen is that you get a recirculation behind the base, even with an inviscid solver. This is due to numerical dissipation, ideally the flow should be at rest. Now a word to the superiority of a viscous computation in such a case. This is still very much subject to research activities and people are starting to get decent results for certain test cases by using very large LES computations. Most, if not all, turbulence models get the pressure in this base region wrong. So I would say that the gain of a computation with turbulence modelling is not high, if not zero.

Read the original question again. Do you really think this is a study on numerical dissipation on Fluent? Maybe so... but I wouldn't bet on it.

Separation is inherently tied to viscosity, whether the flow is subsonic, sonic, supersonic, or hypersonic. Sure, a strong shock, expansion, or a discontinuous shape can help to force separation to occur where it should, but even then your solution will be sensitive to the local interaction between boundary-layer and shock, boundary-layer and wall. I don't doubt that your numerical-dissipation-dominated inviscid flow produces qualitative results that make sense. Flow around an edge separates at the edge -- big surprise (the fact that some people seem to be surprised to see flow separate from the leading edge of a flat plate was what puzzled me into response). But sure, even in less obvious cases, numerical dissipation is of dissipative nature (hence the name), and delivers the qualitative effects. Just don't expect the solution to remain the same when you play around with your artificially assigned "viscosity". Instead, you can expect to get into trouble if you were to minimize artificial dissipation to find a more accurate solution. To get the flow around a cylinder to separate near the shock -- big deal -- but try to get the dissipation rate inside the recirculation region right with an inviscid model, even when the real flow is nicely laminar. To suggest that viscous computations do not offer even the prospect of higher fidelity (and a more accurate depiction of reality) is a hilarious point of view. I don't know any serious CFD expert who chooses Euler over RANS, LES, or even DNS with the claim of higher accuracy. Do you??? CFD Student had his reasons to run Euler, as many other people do. I doubt it was because he thought so highly of it that Navier-Stokes wouldn't have been good enough.

a few comments:

"Separation is inherently tied to viscosity, whether the flow is subsonic, sonic, supersonic, or hypersonic."

I don't think so, check your gas-dynamics book and you will probably agree.

"Flow around an edge separates at the edge"

No, it doesn't always. When does a supersonic flow separate at an edge? Can you predict this with an inviscid model? What do you think?

In certain cases Euler computations give you just as much information as a RANS simulation, but they run a lot faster. Turbulence modelling introduces an additional source of artificial viscosity which can be difficult to control sometimes. In other cases an Euler computation is utter bollocks. I think we probably agree that a DNS would be close to optimal, but if you cannot afford this you need to model the real physics. Which approach is the best varies from case to case and for some cases an inviscid model is not bad at all.

I think that the question is really much more easy.

Numerical discretization will always introduce some additional term; it can be of diffusion, dispersion, dissipation type, depending on the order of the scheme.

So, when applied to the Euler equations, these terms will modify it in such a way that, as stated, will depend on the local grid refinement, order of the scheme, kind of scheme etc.

Now, the question is: these additional terms can produce entropy? The answer is, of course, yes.

The second question is: are there other things that can produce entropy in an euler solution? The answer is again yes, they are the shock waves. The question here is that the Euler solution is not a potential one. That is, on a theoretical basis, it will never produces entropy spontaneously (except for shocks) but it's not irrotational. Instead, downstream of a curved shock wave, there will be a rotational region which is fully compatible with the euler equations.

Finally: knowing this about an euler solution, do i always have to switch to a viscous solver? I think that the answer is no. Obviously we can't expect that the numerical values will be accurate but with some control on the grid (not so much), it can give some meaningful results.

That's all.

About the flat plate...well i feel involved because i've been the one who made this example but i never said that i was surprised by the separation at the leading edge but just that i was not sure about the reason, which is clearly explained in my previous post as my interpretation of the result. Moreover, it was my first CFD simulation, some years ago, and clearly had just a pedagogical target and no kind of research was involved in it.

Hello, Your site is great. Regards, Valintino Guxxi

Just a general observation.

We do some inviscid solutions as an initial step in high speed (mach 5-10) inlet design using GASP. We investigated using Fluent and were forced to come to the following conclusion.

Fluent has no truly inviscid solution. Even when running slip walls with no turbulence, the viscosity of the fluid remains. You can set that value as low as you like but the solver remains a viscous RANS solver.

Additionally we observed some rather odd behaviors. A definite wiggle to the solution at the shocks. An acutally flow reversal at the wall where there are reflected shocks.

So take it all with a grain of salt. Do not expect to get a true Inviscid solution from this tool.

- Andy R