# Boundary Layer created by Euler Solvers

 Register Blogs Members List Search Today's Posts Mark Forums Read

 November 13, 2001, 11:43 Re: Separated Inviscid Flow - A Reference #21 Axel Rohde Guest   Posts: n/a Kalyan, Although I agree with most of your theoretical views on the Euler and Navier Stokes equations, there are a few statements you made that do trigger a response in me (although I would eventually like to close this chapter): As far as I know there are no Euler solvers that actually implement, DS/Dt = 0 They all have some amount of numerical viscosity, which acts as entropy law enforcement. A certain amount of numerical viscosity is a necessity, otherwise you will end up with phenomena like expansion shocks in perfect gases, which are physically incorrect (see above post). So most Euler solvers (at least the ones I know) do have the entropy law 'built in', DS/Dt > 0 "Separated flows, unlike ones with shocks, do not form unique solutions for any form of continuous Euler equations." Steady flows with shocks, I believe, are not always unique, either. If I remember correctly, the supersonic flow over a cone (for certain cone angles) can either form a (strong) detached bow shock, or a (weak) attached oblique shock, depending on the initial conditions present. "The functional forms of Euler and NS equations are different : NS equations are parabolic and Euler equations are hyperbolic." As a programmer, I am only interested in the unsteady Euler and NS equations, because they can simply be marched in time (perhaps there was a misunderstanding). The unsteady (compressible) NS equations, I believe, are a mixed set of hyperbolic-parabolic equations (hyperbolic in time and parabolic in space, I believe, but please correct me if I am wrong). From a numerical viewpoint, both sets of equations are very similar, one is the subset of the other. "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." According to this statement the unsteady separated inviscid flow over my triangular prism, www.microcfd.com/prism.htm would change its character (not only its amount of detail) each time I double the resolution. Yet I do not find this to be the case. I used to run this test a few years ago at a 200x150 resolution and I got a steady wake (due to heavy numerical damping). When I doubled the resolution to 400x300, the wake became unsteady and its character (in shape and time evolution) looks identical to the current 800x600 resolution. I will soon run this test at 1200x900 (1.08 million cells) resolution, and I will bet you the overall picture will look the same. So I am led to believe that the amount of numerical dissipation within each cell approaches a constant level once the grid has reached a certain fineness. I consider it the 'Kolmogorov microscale of inviscid dissipation' (quite an oxymoron... Also, I have run quite a few inviscid codes over slender surfaces (airfoils) with a NO-SLIP condition in place to test the amount of numerical viscosity present in the solver. There is a point where the 'numerical' boundary layer thickness stays the same, no matter how much you refine the mesh. A good Euler code (like TVD) will exhibit virtually no numerical boundary layer or confine it within the first layer of cells. Ideally, an Euler solver should come up with the same solution, regardless of whether you implement a slip or no-slip condition. The same concept applies to shear layers. I have run Euler (TVD) simulations with supersonic jets exiting into a subsonic free-stream where this was actually the case. There was perfect slippage with no detectable shear layer (not one intermediate layer of cells). For an FVS solver (like MicroTunnel) this is not the case, but on the other the code is very robust. Anyway, these are just some of my observations I have made over the years, and I am not sure how they fit in with more classical theory. Again, I am mainly a 'number cruncher', and not much of a theoretician. Axel P.S. By the way, I only use the conservative form of the equations when writing my code, for both Euler and Navier Stokes solvers.

 November 13, 2001, 14:08 Re: Separated Inviscid Flow - A Reference #22 kalyan Guest   Posts: n/a Axel, I agree that it was found necessary in some of the Euler solvers (in Roe's scheme atleast that I am aware of) to explicitly enforce the entropy condition to prevent unphysical expansion fans. In the early days (when I started in CFD with Euler solvers), I was wasn't too afraid of numerical viscosity. However, once you switch to Navier-Stokes solvers, it is hard to digest an explicit entropy condition since real viscosity is supposed to take care of it automatically. Hence, a lot of research has been devoted to developing solvers (mostly incompressible for use in DNS and LES) with minimal numerical dissipation. On the other hand, I agree that the need for kinetic energy preserving schemes (zero effective numerical viscosity schemes) may have been overstated in the context of compressible flows (given the additional problems in dealing with shocks/shocklets, expansion fans etc.). Entropy fix might very well be needed even in DNS or LES, I can't say since I haven't worked on compressible solvers for atleast 7 years. Perhaps it is worth looking into schemes that do not need such fixes (since LES community would be all over it). Regarding you observations about simulations of flows around triangular prisms, it is hard to conclude that numerical dissipation reaches a constant level by using this problem. You have to realize that the prism has sharp edges and the flow always would separates at these sharp edges thus making the solution look grid independent. Try the same procedure on flow around an ellipse and I bet that grid independence is hard to achieve (since there is no point where one can say apriori the flow would separate). Better yet, try the problem that Adrin always seems to recommend, the flow around a circular cylinder. You can not run Euler solvers with a no-slip condition because by adding this condition you are overspecifying your BCs. I am not sure what the results mean. It has been a long time since I have read up on Euler/compressible solvers. Can you suggest a recent review that I can read so that we do not talk past each other in the future.

 November 13, 2001, 14:55 Check your Post processor software! #23 kp Guest   Posts: n/a Your software may be interpolating wall values which assumes them as zero at wall to cell center values.

 November 13, 2001, 20:17 Re: Separated Inviscid Flow - A Reference #25 xyz Guest   Posts: n/a Please note: we only use the Euler Equations to describe the flow when the boundary layer is very thin with no separation. If this is not true, you can not it at all, at least not in the separation zone and the boundary layer.

 November 13, 2001, 22:14 Re: Boundary Layer created by Euler Solvers #26 Jim Guest   Posts: n/a Thanks, but that's exactly what I do.

 November 13, 2001, 22:41 Re: Boundary Layer created by Euler Solvers #27 Jim Guest   Posts: n/a I'll be happy to let you know if I should make it. Well now, I heard from my colleague that he'd seen the same kind of result at some conference, but the speaker mentioned only just that it was due to a "singularity" (the nonsmoothness at the ends of the circular arc). He suggested me to try a smooth bump. I'm working on it. Well, as someone mentioned, maybe we just need to smooth every corner on the boundaries in order to obtain healthy Euler solutions. If that's the case, I think I've learned a very important tip from this exercise. But then again, should we look for a way to overcome it? Well, of course, we can round off every object in real life instead of its computational boundary. And it sounds more practical........

 November 14, 2001, 13:59 Re: Separated Inviscid Flow - A Reference #30 kalyan Guest   Posts: n/a There are only two kinds of drag that I know of as inviscid drag components, the transonic drag (resulting from shock like phenomena which invariable result only in the presence of viscosity but can be captured using Euler equations) and induced drag associated with finite wings (which result once again from Kutta condition that is once again facilitated by viscosity even if inviscid equations are used). So, theoretically there is no such thing as inviscid drag. If you get drag in inviscid flows, I think the energy conservation would be violated. If inviscid flow around a cylinder causes drag, then consider the case where the air/medium is stationary and the cylinder is moving. Since the drag is non-zero, a finite amount of work needs to be done to move the cylinder at finite speed. This is irreversible work and indicates the presence of a non-conservative force field (i.e., dissipation in the system) which would violate the inviscid energy conservation equation. If there is no viscosity in the system (real or numerical), where is the work going ? I am not an expert on TVD schemes, but my impression was that TVD schemes are pretty dissipative. Is there such a thing as a TVD scheme that is free of numerical viscosity (TVNI maybe).

 November 14, 2001, 14:12 Re: Separated Inviscid Flow - A Reference #31 kalyan Guest   Posts: n/a Axel, CFD is indeed a great learning tool. But before we claim that it has predicted a phenomena yet undiscovered or paradoxical, isn't it incumbent on us to see whether the predictions are real or numerical. In order to judge the CFD predictions, ones needs good knowledge of fluid mechanics first. Once the CFD solutions are verified and validated, then I agree that they can be pretty educational. DNS does provide a window into the physics of turbulence. However, some in the LES community have learnt the hard way not to base their model development on DNS results (an approach called apriori analysis). Models based on such analysis are no longer accepted in the current day unless they are validated by other independent means.

 November 18, 2001, 00:18 Re: Boundary Layer created by Euler Solvers #32 Jim Guest   Posts: n/a Hi, My colleague was right. I use a smooth bump (A*sin(pi*x)), then that funny wake disappeared. I have nice symmetric Mach contours now. Jim

 Thread Tools Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post tomyangbath FLUENT 17 March 25, 2016 05:36 ARC Open Source Meshers: Gmsh, Netgen, CGNS, ... 0 February 27, 2010 11:56 Luk CFX 3 February 27, 2009 04:22 michele OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 2 July 15, 2005 04:15 Wen Long Main CFD Forum 3 September 24, 2002 08:47

All times are GMT -4. The time now is 23:15.