Hi, I have a simple question: Can you completely eliminate boundary layers created by Euler solvers? (of course, on a grid of a reasonable size. not h->0)

I computed a low-speed subsonic flow over a small bump on a structured nearly uniform quadrilateral grid by a 2nd order MUSCL-type finite-volume Euler solver with Roe's flux formula, with pressure extrapolation on the solid boundary (flux=[0,p*n,0] on the wall). In the solution, I see a boundary layer behind the bump, i.e. the x-velocity decreases towards the bottom wall (not goes to zero, though); all other variables look symmetric wrt the bump.

Well, is it a nature of Euler solvers? I want to know whether this is just a limitation or a bug.

Thanks, Jim

Can you specify your 'bump' a bit further? Is it a smooth bump, or a sharp one? Even with an Euler code and no 'boundary layer resolution' (the term makes no sense if you implement a slip velocity condition), you can get recirculation after a backward facing step (sharp corner). This has nothing to do with 'boundary layer' separation.

Thank you for your response.

The bump is circular with 5% thickness wrt its chord. So, it is not smoothly placed on the bottom wall, I mean, if in a supersonic flow, there will be a shock rather than an isentropic compression wave at the left end of the bump.

Right, the word "boundary layer" does not make sense because I implementy a slip velocity condition on the solid boundary. Let me explain my result again. Behind the bump, if I plot x-velocity (or U) versus y axis, U is almost constant but it decreases rapidly near the bottom wall to a smaller value (it looks like a typical velocity distribution across a BL except that the velocity is not zero at the wall but a small finite value: it does slip. ). If I plot the contours of U, it is not perfectly symmetric, contours become parallel to the bottom wall behind the bump. So, the trend continues to the right end of the domain. I get this even if I used a very fine mesh (600x300 cells). I don't know what this is. Does anybody know? Does anybody get similar results?

(BTW, on the outflow boundary, I place ghost cells with freestream values, and let the Roe scheme extract the necessary information for me.I think this is not a problem.)

I am still not totally clear about your results, but you cannot expect a (perfectly) symmetric (velocity) profile with respect to the bump when using an Euler flow solver. Another example, compute the flow around a circular cylinder using your code. You will notice that the profile will become more asymmetric as you increase the Mach number. Even for a fully subsonic flow (no local regions with M > 1, i.e. a shock free flow), your 'inviscid' drag will increase with Mach number. Don't confuse inviscid compressible (Euler) flow with potential flow. - What is your flow Mach number by the way?

Hi,

I am just guessing that maybe the "boundary layer" is generated by the "slip velocity" you specified on the symmetric plan. For an invicid flow the velocity gradient (or shear) dU/dy = 0 @ wall (I guess again this is what you are looking for). When you impose a slip velocity that does not "go well" with the free stream velocity, the velocity profile near the wall has to be "adjusted" to satisfy the velosity boundary value @ wall and there you have your "artificial" boundary layer.

I hope this helps.

Thank you again for your comment.

I see what you say. But the Mach number i'm talking about is 1.0E-02 (I should have mentioned this, sorry), so it is almost potential flow, and therefore I expect a symmetric solution.

What puzzling me is the fact that I don't get a clean potential flow solutions even on a very fine grid. The discretization is not consistent?

I'm doing some literature search, but so far I haven't found anything relevant yet.

Thank you for your comment.

I guess you're right. So, there may be a better wall boundary condition. I tried also a reflective bc in which I place a ghost cell and specify the state (same density, pressure, and tangential velocity, but normal velocity is flipped so that the sum of this and that of the inner cell becomes zero), but I find no big difference.

I wish I could fix the Mach number on the wall. But it just doesn't seem a correct boundary procedure. Plus, it is not constant along the bottom wall all the way, it has some variation near the TE of the bump.

The proper boundary condition on the wall for Euler is a zero normal velocity. So apply mirror cells in which you impose: say your first cell on the boundary has index i and your mirror cell (in the solid) has index i-1 than you have to impose U(normal to wall)i-1 = -U(normal to wall)i U(tangent to wall)i-1 = U(tangent to wall)i Pressure i-1 = Pressure i Density i-1 = Density i

The reflective B.C. is the one I use in my computations when running Euler code. Most Euler solvers become inaccurate at M < 0.1, so if you are running at M = 0.01, then don't be surprised if your answers are not 'perfect'. I have never run a MUSCL code (only different types of FVS and TVD), but if I remember correctly, there are a few MUSCL codes that use preconditioners to run at such low Mach numbers. Did you write this code yourself? Does it have a preconditioner?

This may or may not help you, but I have run a TVD solver for flow over a circular cylinder in the past (inviscid) and at M < 0.3 (and eps = 0) I always see a 'boundary layer type' effect near the surface. The problem goes away when I increase the numerical viscosity parameter epsilon ( 0 <= eps <= 0.5 ).

Technically, the inviscid flows can not separate. Any separation caused by Euler solvers is a numerical artifact.

Well, we are talking CFD, aren't we? - And I used the word 'recirculation', which does not imply 'boundary layer' as the word 'separation' does. 'Technically' speaking, yes, the recirculation is due to the numerical viscosity which is present in any 'inviscid' flow solver. Physically, this feature or 'artifact' is desirable, otherwise we could not study inviscid flow over airfoils, either. The rearward stagnation point would not coincide with the trailing edge of the airfoil at non-zero lift, and we would have to reinforce the Kutta condition the way we do in potential flow, by adding the right amount of circulation, which is not known a priori.

Here (once more) a nice example of an unsteady, 'inviscid' wake with recirculation (not to mention the periodic shedding of transonic shocks),

www.microcfd.com/prism.htm

My point is this: Why bother with computationally expensive Navier-Stokes solvers and 'turbulence' models, if a simple inviscid solver can capture virtually all the desired physics of a (particular) flow.

Collela developed a classical method to dealing with the singular point in the back-step Euler flow. It works well for that case. Sorry but I can not remember the location of journal.

I searched through my old notes and finally found a paper on separated Euler flows:

"Euler Solutions as Limit of Infinite Reynolds Number for Separation Flows and Flows with Vortices"

By Wolfgang Schmidt and Antony Jameson, p.468-473 (sorry, can't tell from the photocopy who published it)

I am going to take the liberty and quote the conclusion here:

"The paper has presented an efficient solver for the full inviscid time dependent compressible Euler equations giving solutions in two- and three-dimensional flow with separation. It has been shown that this type of separated flow can occur on both round surfaces and sharp corners. In all cases compressibility is needed to allow for these solutions. All these results raise the question of the comparison between the exact inviscid solution and the limit of Navier Stokes solutions if the Reynolds number is increased to infinity."

So the keyword here is compressibility!!!

Well, I am glad I am not alone in my 'separated' inviscid computations. Obviously, Jameson's results have a little more weight than mine...

Here another quote from the same paper:

"Due to compressibility any flow around the corner would produce a shock such that the only possible solution in the converged steady state is the one with the flow leaving the corner."

So recirculation or 'separation' in Euler flows at a backward facing step is not merely a 'numerical artifact', although the phenomenon is aided by numerical viscosity which suppresses entropy violating expansion shocks in perfect gases (in real gases expansion shocks are possible).

Expansion shocks are not possible for real gases are they? If so, why? Wouldn't that violate the second law of thermodynamics?

Martin

Thanks. Yes, I do use preconditioner (the one developed by Van Leer et. al.), which is supposed to work well for low speed flows.

Now, your comment below could be of importance. The use of a preconditioner requires the artificial viscosity term to be modified for some schemes including Roe's. So i did it, but there may be a bug. I'll look into it.

Thanks again.

I don't know too much about expansion shocks in real gases (although I have erroneously computed a few myself in shock tube flow for perfect gases), but I can quote an excellent reference here, a book, which anyone studying CFD should read at one point,

"Computational Gasdynamics", Culbert B. Laney, Cambridge University Press, 1998

Let me take the liberty to quote a paragraph from p.43:

(Bert, if you read this, maybe you can jump in and EXPAND on this topic...pun intended..

"Real gases may reverse the shock relationships. For example, in a real gas, shocks may decrease rather than increase pressure and density - this is called an expansion shock. However, although the nature of the fluid as specified by the equations of state may affect other aspects of shocks, the second law of thermodynamics always requires that the wave speed just to the left of the shock must be greater than the shock speed, which must be, in turn, greater than the wave speed just to the right of the shock."

(The direction of the flow in the above discussion is from left to right)

So, yes, expansion shocks are possible in REAL gases.

Let me know how you made out. I could definitely use some feedback on this topic. The 'boundary layer effect' for my TVD solver at Mach < 0.3 and epsilon = 0 turned into a real dilemma, when I tried to do a viscous computation - the inviscid TVD solver was the core of my Navier Stokes solver. When I increased epsilon, the dimensionless parameter that controls the numerical viscosity of the TVD solver, the inviscid solver was working correctly, but as a result, my actual viscous boundary layer, which developed as part of the overall NS solution was smeared, as physical and numerical viscosity approached the same order. In essence, I could not get a good NS solution below Mach = 0.3, because with or without numerical viscosity I had a problem.

Did anyone else ever run into this problem?

Separation and shock are strictly possible only in the presence of viscosity. However, the flows across the shock (not the internal shock layer) satisfy the inviscid equation when written in a conservation form.

In CFD, if your boundary conditions are such that the only steady state solution is one with a shock, a shock is created. Since shocks do satisfy discretized conservative forms of Euler equations, the shocks are sustained (stable). As many of us know, non-conservative forms of Euler equations do not create shocks. This is because non-conservative forms are differential forms which do not accomodate shocks.

There is however a subtle point to be noted. Euler equations can not generate entropy. So the substantial derivative of entropy is zero in Euler flows. Some times this equation replaces the energy equation in computations. However, when we want to capture shocks, we relax this condition by saying that entropy can increase but not decrease (a condition which we know from physics with otherwise no mathematical significance).

In summary :

DS/Dt = 0 for Euler flows (shocks can not be accomodated as solutions).

Euler flows with DS/Dt > 0 (relaxed equations) : shocks can be part of solutions.

Now getting back to separation, separation has to do with viscosity. Separated flows, unlike ones with shocks, do not form unique solutions for any form of continuous Euler equations. The functional forms of Euler and NS equations are different : NS equations are parabolic and Euler equations are hyperbolic. Also, the wall boundary conditions are different. Therefore zero viscosity limit of viscous flow never equals inviscid. If you use Euler equations and predict separation, this separation is aided by numerical viscosity which as we all know depends on grid spacing. As we refine the grid, the numerical viscosity keeps shrinking and the separated solution keeps changing. There would be no grid independence and Lax condition would be in violation.

I am not sure what to make of Jameson's work since his contributions to CFD have been tremendous but it is worth noting that he made his living using Euler solvers and MG methods.