I am testing an inlet diffuser, say inlet of Ramjet, with inviscid code based on Roe scheme.

The specification of test case:

The altitude I choose is 6000 meter, which corresponds to p_inf=2.8 kpa and Mach_inf=3. For a specified back pressure equal to p_back=28 kpa, I get multiple oblique shocks and a terminating normal shock downstream of the throat and the code converges properly.

The converged solution is a correct physical solution, as far as I could check by verifying the conservation equations for a control volume taken around the whole inlet.

The normal shock for this back pressure is not located at the throat and it is further downstream. So what i do, I gradually increase the back pressure to 30 kpa (I use the result of converged 28 kpa as initial condition). Then what happens is as follows:

1) If I use a third order upwind biased, a circulating region at the exit plane starts and moves upstream while it grows until the code totally diverges.

2) If I use first order, the normal shock moves upstream until the shock disgorges out of the inlet, making a shock like a bow shock, then the shock is swallowed by the inlet again. This procedure is repeated forever. I am doing inviscid flow analysis, so I am sure the oscillation has nothing to do with inlet buzz.

I wonder if you can help on this problem to give me some hint in finding the source of instability in my code. I have benchmarked the code for many internal and external cases.

Is any way that I can check the specified back pressure for this geometry, has a physically possible solution at all for this mixed supersonic-subsonic? Have you ever had such a problem before?

If needed please let me know to send you some pictures about the geometry and the procedure that the solution evolves with time.

I know my e-mail was too long. I am so sorry about it.

Thanks a lot for your help.

Regards,

Mohammad Kermani

Dear Mohammad, It seems you're in big trouble isn'it ? Did you verified that the back pressure isn't too high ? Anyway you could send me some picture , with that I could help you more. (Finally in two days I'll be home !) Bye.

Although you are solving for the Euler equations, you are necessarily introducing artificial dissipation to obtain a numerical solution, which acts as viscosity and makes your discretized Euler equations behave as Navier-Stokes. What you are observing might indeed be an inlet buzz, but a faked one caused by the artificial diffusion introduced by your discretization scheme.

By the way, do you use an entropy satisfying parameter along with your Roe scheme, and if so, what value do you give to it? I suggest running your case with and without the added artificial dissipation induced by the entropy satisfying parameter and compare results..

And again I'd caution in analyzing an Euler flowfield obtained through CFD means as a real Euler solution, but rather as something in between Euler and Navier-Stokes, again due to the issue of artificial dissipation.

-bernard

(1). A very good point indeed.

Hi Bernard,

For the inlet buzz, I think this is not due to the inlet buzz. Because I am using Roe scheme and the artifical diffusion are very small. Moreover, I am just using structured grid, in which most of the flow is almost aligned with the grid, so the artificial diffusion caused by grid obliquness are also small. So it doesn't look to me an inlet buzz problem.

For the artificial diffusion I use:

lamda <-- (lambda^2 + eps^2 )/(2 . eps)

where eps = 4 max[0, (lambda - l_L), (l_R - lambda)]

The band for eps I use, is four times wider than what Harten-Hyman has introduced. (Harten-Hyman's is: eps = max[0, (lambda - l_L), (l_R - lambda)] )

l_L= lambda_L

l_R= lambda_R

thanks

M

By artificial dissipation I don't only refer to the dissipation added through the entropy correction terms, but rather to the overall artificial dissipation of your flux discretization scheme. The Roe scheme has some artificial dissipation built-in which you can't get rid of. The circulation region that you are obtaining proves that there is an important amount of artificial dissipation present since this type of viscous dominated flowfield should appear only when solving Navier-Stokes flows.

The entropy correction terms increase however the artificial dissipation and, by turning it on or off, it is possible to get a feel of just how much artificial dissipation is influencing the solution.

-bernard

As far as i know, Roe scheme is totally non-diffusive for grid aligned flows. This can be checked by having two parallel straems with different Mach numbers, say 2 and 4. If inviscid flow, the discontinuity of this slipline is captured within two nodes, exactly like analytical. This shows Roe has no artifitical diffusion in itself. The artificial diffusion added is either due to entropy correction or grid obliquness.

Thanks

Mohammad

It's not because the scheme behaves as being artificial-dissipation free for one particular case that in will always be. The Roe flux at the interface can be written as:

F_{i+0.5}=0.5*(F_i+F_{i+1})-0.5*|A_{i+0.5}|*(Q_{i+1}-Q_i)

where there is no doubt that the second term on the RHS is second-order artificial viscosity which may vanish for some particular problems but is generally present for common flows.

All schemes discretizing the Euler equations must introduce artificial dissipation at one point or another. Such artificial dissipation does not need to be in the form pointed out above: even an exact Riemann solver, for example, will introduce high amounts of artificial dissipation for 1D flows.

For the Navier-Stokes equations, however, it is possible to have an artificial dissipation free discretization for the convective terms but only at very low Peclet numbers where the physical viscosity will be high enough to stabilize convective processes. To attain such low Peclet numbers however, the grid would need to be of substantive size hence requiring high computing resources, which is why most of us lean back on artificial dissipation to get an answer. Special care must however be taken and results must be analyzed cautiously.

At the risk of repeating myself, I again point out that a circulation zone is not possible in the Euler equations and is hence a proof of the high amount of un-physical diffusion present in the flux discretization method you are using.

-bernard

Hi.

In an upwind scheme, the values at the left side and right side of the cell face are determined. As the gap between these L and R values increase, the numerical diffusion introduced by the scheme increases. (an example, the idea of making the scheme higher order is in order to reduce the gap between L and R => reducing the numerical diffusion).

In Roe scheme, after the L and R conditions are determined, ONLY a single condition is specified to the cell face, i.e. the gap between L and R becomes zero. That is Roe's averaged condition is only referred to the cell face and not L and R, although it is determined w.r.t to L and R conditions. That is, the reason, which makes the Roe scheme a non-diffusive scheme.

Thanks

Mohammad

(1). We are just trying to point out some of the possible reasons why you said you are having problems. (2). In addition to the possible numerical diffusion (it doesn't matter whether it is there or not right now, because it is a possible source of problem), the downstream exit boundary condition also will cause the wave propagation upstream. (3). Inlet buzz has been studied by using transient Navier-Stokes equations in the past, so, you may want to review the AIAA Journals or papers. (4). By the way, flow oscillations have been numerically observed in the inlet buzz, stagnation point cavity many years ago.

Artificial viscosity is not so high to induce such an instability, and certainly not enough to produce a buzz effect. This doesn't mean that an Euler solution is a really non-viscous solution, but rather than that discrepances between those two cases are not so high to induce a typical viscous effect (buzz!). I do still think that your problem is dued to an ill-posed boundary (outlet) condition (i.e.: outlet pressure too high!). To analize this I should have at least the on-design values of variables and your test values ; as for picture I'd like to view a zoom on the cowl lip (shock to shock interaction) and a general view of the flow-field (pressure contours ?) with the grid superimposed. Without these elements nobody can help you further.

Inlet buzz at supersonic speeds is generally an inviscid interaction, and the Euler equations are an adequate level of modeling to capture supersonic buzz. From the qualitative information you have conveyed, your solution seems plausible.

Ray,

Could you possibly introduce me some reference in which inlet buzz is captured by inviscid flow simulations.

Sofar, if you check previous postings, we were thinking it is ONLY a phenomena in viscous world.

Although there were some references, like AIAA education series due to (1) Seddon and (2) Mahoney, but non of them are talking about whetaher inlet buzz is for inviscid or viscous?

Thanks

M

Are you joking!

(1).Buzz (in a supersonic inlet) is a low-frequency, high amplitude pressure oscillation that is linked to shock/boundary layer and/or/shock/shock interaction at "relatively low inlet mass flow ratio". (2). As an example, consider the external compression inlet, operating in the "subcritical regime"(flow in inlet not chocked, because the flow is subsonic),the terminal normal shock (outside the inlet) will impinge on the "boundary layer" formed along the wall of the ramp causing "the boundary layer to separate"(shock/boundary interaction is viscous phenomenon). (3). If the separated boundary layer produces a large enough low-velocity flow region (behind the shock and into the inlet), (displacement effect of the boundary layer), the inlet will choke , reducing the inlet mass flow rate and moving the normal shock forward(expell the shock further away the inlet) along the ramp.(lower mass flow rate through the inlet means larger effective body, thus larger shock stand-off distance from the inlet. With zero mass flow rate through the inlet, the inlet becomes a solid blunt body) (4). Since the boundary layer at this forward location is thinner, (closer to the leading edge of the ramp), the separated flow region does not chock the inlet. (thinner boundary layer produces thinner separated boundary layer after the normal shock/ boundary layer interaction.) (5). Thus, the inlet mass flow increases, moving the normal shock back up the ramp toward its original location. This process is repeated again and again, creating "buzz". (6). Ref. PP-380~381, Aircraft Engine Design, by Jack Mattingly, William Heiser, Daniel Daley (US Air Force Academy,Colorado Springs), AIAA Education Series,(1987). (note that supersonic inlet technology is mainly related to fighter aircrafts, except for the retiring Concord supersonic civil transport.)

(1). In old days, propulsion aerodynamics people (internal aerodynamics: inlet, diffuser, nozzle and integration) simply do not talk to the Aerodynamics people (external aerodynamics: wings, fuselage, airframe) (2). So, it is likely that the message came from the external aerodynamics side.

There are many dynamic mechanisms that can occur in an inlet - buzz, hammershock, unstart, stall/stagnation, etc. None of them are simple mechanisms, and each of them has different modes and manifestations.

"Buzz" refers to a periodic shock motion, typically with frequency from a few dozen to a few hundred Hertz. This periodic motion is a coupling between the inlet shock system and the inlet mass flow rate. Basically, when a normal shock forms ahead of the inlet, then the buzz interaction can be initiated. This occurs if the inlet throat is choked, or nearly choked, at the condition in question, and then a normal shock is formed instead of the desired oblique shocks. Due to the added total pressure loss through the normal shock, the inlet now cannot pass the previous mass flow (prior to forming the normal shock). The inlet chokes, the inlet mass flow drops, and the normal shock moves forward from the inlet. As the shock moves forward, progressively more air is now able to spill over the edges of the inlet lip, and the mass flow through the inlet is reduced. This progresses to a point where enough air is being spilled that the inlet now can pass the mass flow passing through the shock system, and oblique shocks can be re-established. The flow recovers, and the process repeats.

As I have described it, this is an inviscid phenomenon. The original trigger causing formation of the initial normal shock may or may not be inviscid (usually it is inviscid) but once the periodic cycle is set up the interaction depends only on inlet geometry and shock characteristics. Analyses based on the Euler equations have proven capable of capturing this phenomenon.

Buzz is a well-known phenomenon associated with inlets operating at a supersonic overspeed condition. It often sets the top speed on military aircraft.

I cannot say if the flow interaction you are capturing in your solutions is truly a valid prediction of buzz. My original comment to you was that it *could* be qualitatively correct based on the limited information you provided, even though you are solving an inviscid set of equations.

My credentials:

Ph.D. in fluid dynamics from California Institute of Technology. 26 years experience in developing and using CFD for aircraft design applications. Currently leading the CFD program for the Boeing company. Prior to this assignment, and prior to the Boeing - McDonnell Douglas merger, 22 years working on fighter propulsion systems for McDonnell Aircraft Company. Projects I have worked on include F-15, F-18, A-12, NASP, YF-23.

No, I'm not joking. Perhaps you are confusing the terminology for different types of inlet dynamic interactions.

(1). The question is really : Have you developed and used the inviscid CFD code to predict the inlet "buzz"? And where is the reference of that results? (2). I have seen the inlet "buzz" predicted by CFD code about 15 years ago, using Navier-Stokes code. And if the inlet "buzz" could be predicted by using Euler code, the it would have been used 15 years ago, because the Euler code is much easier to solve (relative to the Navier-Stokes code ) in those days. (3). Now,this inviscid code is getting something like "buzz" , we are interested in knowing whether Euler code could predict it or not. It is a rather simple question.

Yes, we have used inviscid codes to predict buzz. It is very easy to mistake this for a limit cycle oscillation due to a problem with the code - the key is to examine the Mach numbers in the flow field and see if there is a choke point.

Also have used Euler analysis with good results for other types of inlet dynamics such as hammershock, and unstart. The trigger mechanisms are very complex, and often they involve interactions which we cannot model with CFD today. Example: hammershock generally is triggered by a stall or partial stall in the first or second stage of the engine's compressor. No way can we model that with CFD, including the aircraft/inlet system also. So, we often have to assume the presence of the trigger (i.e., no flow through a portion of the compressor face) and begin the calculation at that point.

Unstart is often triggered by a boundary layer separation which constricts the aerodynamic internal flow passage to the point where it is choked.

But once the interaction is triggered, Euler solutions do a very fine job in capturing the essential issues such as overpressure and the impact of control or mitigation design strategies. These flowfields (inlet dynamic phenomena) are dominated by transient behavior of shock waves, and viscous interactions set up too slowly to impact the first-order character of the interactions.

There is no reference I can provide to you, unless you are a Boeing employee. Sorry.

Since I work in aerospace industry, we generally do not publish our work, especially when it pertains to real or proposed aircraft. We publish about 1% of our work, and then only for simple problems. Usually we have a business objective in mind when we do publish. As far as professional advancement is concerned, publication is irrelevant and so we in industry generally publish very little. Preparing a good paper is a lot of work, and it has at best only a marginal impact on your advancement. Further, there are always issues of disclosing company goals and capabilities by premature publication of data. The work of which I am most proud has never been published and probably never will be.

Mr. Taurchini's description of buzz based on ingestion of a vortex sheet is another common interpretation of the phenomenon. That was the explanation that I was given when I was a junior engineer (more than 20 years ago). However, I think I am in the mainstream of current thinking when I interpret the physics in terms of shock losses (oblique vs normal) and choking. The two interpretations are overlapping to a degree, since a vortex sheet is always present at the intersection between the normal and oblique shocks (during the growth phase of the buzz cycle).

There is always the possibility that the periodic solution which was the root of this thread is due to numerical issues, and is not actually a representation of buzz. I don't think any of us can give a high-confidence answer to that question without examining the 3-D unsteady solution. My input to this thread is that the solution *could* be qualitatively valid, based on the information which was presented at the beginning of this thread.

Even if we assume that the solution in question is a valid representation of buzz, I certainly acknowledge numerous issues such as artificial viscosity and phase errors which degrade the accuracy of predicting a propagating wave. As an example, for certain combinations of algorithms and grid stretching, we actually can make a shock wave stop, and reverse direction incorrectly (that one we published - AIAA paper, 1993, authors are Bush and Cain). So, even if the solution is plausible, I don't think it can be considered to be more than qualitatively correct.