What about angular momentum conservation?

We usually solve the equations of mass, linear momentum and energy. So why not angular momentum?

Is it not important or is it dealt with by the general Navier-Stokes equations. If not, why is the solution of angular momentum not included in the formulation??

Thanx for your time

Barry

It is implicitly included in the Navier-Stokes equations.

If you check a book on classical physics you should have no problem to find a derivation of the conservation of angular momentum based on energy conservation (force normal to velocity).

For swirling flows where the exact numerical conservation of angular momentum is considered important one can modify the differencing to numerically conserve angular momentum instead of the physical velocity components. This can be important for strongly swirling flow with significant changes in radius.

A good explanation about the conservation of angular momentum and symmetry of the stress tensor Tij is given on pages 119-121 of the book

Incompressible Flow Ronald Panton John Wiley & Sons 1994

Basically, if the microscopic angular momentum is randomly oriented, then the stress tensor Tij is symmetric, and in this case, the angular momentum of a continuum fluid is no longer independent of the linear momentum equation (ie, you can derive the angular momemtum equation of the fluid from the linear momentum equation).

I couldn´t help sending this message. I´ve been working on the LES of a hydrocyclone and I have come to interesting conclusions. If the first-order upwind scheme is used, the swirl velocity profile seems to better adjust the experimental results. If the second-order central scheme is employed (in the few cases in which convergence was reached), the profiles depart from the experiments and are lower than those computed with the first-order upwind. This sounds incoherent, since the numerical diffusion tends to smooth gradients so as to reduce the magnitude of the velocity. I attribute this to the lack of conservation of angular momentum and I´d be grateful if you suggested something I could do to avoid this.

Best regards,

Francisco.

What do you mean by non convergence of an LES method?

LES and first order methods? I do not know what you are doing but this sounds seriously wrong.

LES is all about getting accurate convection terms - adequate resolution is absolutely essential in order to get sensible results from an LES run in a way it is not for a RANS prediction. If your grid resolution is inadequate one usually experiences too much turbulent transport and overly anisotropic Reynolds stresses.

Numerical diffusion is rarely important in a normal LES run because the levels of diffusion have to be small for an LES simulation to make sense.

If you are using a collocated scheme with pressure smoothing then dump it and switch to grid staggering. The presence of strong radial pressure gradients will almost certainly be introducing signficant nonsense terms via the pressure smoothing. If this is not an option you could try to back out the effect of the mean radial pressure gradient in some way.

It seems unlikely to me that the conservation of angular momentum is at the heart of the problem. Nonetheless, it is easy to rearrange the convection terms so that angular momentum is conserved exactly at all times. For a highly swirling flow this is probably a wise thing to do anyway.

Yes, I´m aware of these facts. What really suprises me is that the results are in good agreement with the experiments when the upwind scheme is employed. I would like you to visit my homepage and see it for yourself: www.geocities.com/chicao99br. When I say non-convergence, I mean that the simulation blows up (the central scheme is way too unstable) and perhaps the grid should be sufficiently refined. I´m now preparing an animation with the 3D simulations in which the structures and turbulent patterns that actually occur inside a hydrocyclone can be easily seen.

It certainly looks like an interesting flow.

If you get good agreement using an upwind scheme which you know contains large incorrect terms then I would suggest they are cancelling other large errors from other terms. One explanation may be that they are clobbering excessive turbulent motion due to inadequate grid resolution. You would have to look closely at your solution for confirmation or not. About the only thing one could say for sure is that things aren't right when this happens.

Why is the central scheme stability an issue? (what's your Courant number?).

What do the Reynolds stresses look like? These are often the best indicators of inadequate resolution.

What/where is you exit condition? This is a source of stability problems for many strongly turbulent LES flows.

Why aren't you worried about the asymmetry in your mean flow plots? Wouldn't you expect any precessing to average out over the length of the simulation? or does it have something to lock onto?

I´m glad to discuss these issues. As far as I know, the spacial stability limit for the central scheme is Pe<2 and the problem is that the Pe for most cells in my grid are much higher than that. Actually, I was able to use the central scheme in my 2D axisymmetric simulations, since I could refine the mesh enough. But for the 3D case, even with very small time steps, the simulation blows up. In order to attempt to simulate the same conditions in which the experiments were carried out, I imposed flat axial velocity profiles at upper and lower exits so as to allow 80% and 20% of the inlet flowrate to leave the cyclone. I know this may not be the best, but no other experimental information is available. About the asymmetry in the plots, this is expected, because the inlet the flow enters on one side of the vertical axis only. Actually it tends to become nearly symmetric as it enters the conical region (this is known from experiments). It is known that in flows of this nature, the tangential is the highest component, and it roughly distributes as coaxial cylinders. This flow is also known to be anisotropic, with the resistance to radial flow much higher than that to axial flow. If you´re willing to know more about this flow, I could number a few references.

Best regards,

Francisco.

>> As far as I know, the spacial stability limit for the central scheme is Pe<2 and the problem is that the Pe for most cells in my grid are much higher than that.

You are performing an unsteady LES simulation not a steady RANS prediction. I would suggest you check your stability limits for convection and diffusion (the centre line is classical problem here) and how they relate to the required time step to perform an accurate simulation through time. What method are you using for your time integration?

>> In order to attempt to simulate the same conditions in which the experiments were carried out, I imposed flat axial velocity profiles at upper and lower exits so as to allow 80% and 20% of the inlet flowrate to leave the cyclone. I know this may not be the best, but no other experimental information is available.

I think this means you are injecting a jet with zero turbulent energy. Is that reasonable for your test case? What happens to the turbulence and mean velocity profile in the vicinity of the exit?

>> About the asymmetry in the plots, this is expected, because the inlet the flow enters on one side of the vertical axis only.

OK. I had misunderstood why you considered an asymmetric flow a good sign.

>> If you´re willing to know more about this flow, I could number a few references.

Thanks for the offer and I would be interested if there are reasonably detailed measurements of the turbulence field.

For the time integration, I´m currently using the second-order Adams-Bashforth scheme for both convective and diffusive terms, but I´ve also tried the Crank-Nicolson for diffusion. You've mentioned something interesting about the B.C.´s. Actually, I´m injecting a jet with zero turbulence energy and since at the exits the profiles are uniform, they contain no turbulent kinetic energy. It is easy to see in the time animations that the instantaneous velocity profiles don´t fluctuate in the vicinity of the exits and inlet. Also, when I employ the central scheme, it is in these places that the speeds are overpredicted, which in turn cause to simulation to blow up. Should I superimpose some white noise on those profiles in order ot overcome this? Unfortunately, references on hydrocyclone flow are scarce and practically contain no information on the turbulence field (usually only mean components). Anyway, below are some interesting ones:

Dabir, B., 1983, "Mean Velocity Measurements in a 3"- Hydrocyclone using Laser Doppler Anemometry", tese de Doutorado, Chemical Engineering Department, Michigan State University, East Lansing, MI.

Dyakowsky, T. and Williams, R. A., 1993, "Modelling turbulent flow within a small-diameter hydrocyclone", Chemical Engineering Science, Vol. 48, n. 6, p. 1143-1152.

Frank, T., Wassen, E., Yu Q., 1998, "Lagrangian Prediction of Disperse Gas-Particle Flow in Cyclone Separators" Third International Conference on Multiphase Flow - ICMF'98, Lyon, France, 1998 CD-ROM Proceedings, Paper No. 217, p. 1-8.

Hsieh, K. T. and Rajamani, R. K., 1991, "Mathematical Model of the Hydrocyclone Based on the Physics of Fluid Flow", AIChe Journal, Vol. 37, n. 5, p. 735-745.

Malhotra, A., Branion, R. M. R. and Hauptmann, E. G., 1994, "Modelling the flow inside a hydrocyclone", The Canadian Journal of Chemical Engineering, Vol. 72, p. 953-960.

Meier, H. F. and Mori, M., 1999, "Anisotropic behavior of the Reynolds stress in gas and gas-solid flows in cyclones", Powder Technology, v. 101, p. 108-119.

Meier, H. F., Kasper, F. S., Peres, A. P., Huziwara, W. K., Mori, M., "Comparison between turbulence models for 3-D turbulent flows in cyclones", proceedings XV COBEM.

nice websites: http://www.psl.bc.ca/equipment/hydrocyclone http://www.tu-chemnitz.de/mbv/TechnT...on/zyklon.html

Best regards,

Francisco.

>> Also, when I employ the central scheme, it is in these places that the speeds are overpredicted, which in turn cause to simulation to blow up. Should I superimpose some white noise on those profiles in order ot overcome this?

So long as the flow does not laminarize, white noise + flat fixed profile is unlikely to be much of an improvement since it will fairly rapidly disappear. What is often required is a reasonable inlet length for "real" turbulence to evolve after some simulated artificial inlet turbulent condition. Of course, this is only necessary for cases where the inlet turbulence signficantly affects the flow in the working section. I do not know if this is the case for your flow or not.

The exit condition for highly swirling flow is going to be important because changes here will affect the whole field which is not the case for most flows. The use of a fixed flat exit profile may be stable but is going to be very hard to defend as physically reasonable (because it is not). For LES you really need to be using a form of convective exit condition which allows turbulence to convect out with little distortion. And for a swirling flow you ought to let the mean swirl and axial exit profiles develop. A short exit length may also help if you do not have one (not sure from the vector plot). Truncating all backflow is probably going to be necessary as well.

Dear Andy,

after some modifications in my code, I have been able to compute the hydrocyclone flow with the central scheme. Several instabilities which resemble those in wavy Taylor-Couette flows have appeared and this is far more realistic than the solution with the upwind scheme. I used the upwind solution as the starting point for the time realizations with the central scheme. The turbulent structures develop as the calculation proceeds, but after some time, the axial velocity takes very high negative values where its average should be positive (fluid flows upward next to the wall, where it is expected to flow downward). This evolves, inverting the rotation direction of the turbulent structures which were physically sound and eventually the simulation blows up. Do you think this might be related to the initial field? By the way, I´ve just found a paper that contains data on the turbulent flow field in hydrocyclones (you can get it at Science Direct):

Flow patterns in conical and cylindrical hydrocyclones

B. Chiné and F. Concha

Chemical Engineering Journal 80 (2000) 267-273.

Thank you in advance,

Francisco.

>> This evolves, inverting the rotation direction of the turbulent structures which were physically sound and eventually the simulation blows up. Do you think this might be related to the initial field?

Unlikely. I would anticipate problems with the exit boundary condition but if the problem is originating on the wall I would suggest studying the pressure smoothing.

If you are using pressure smoothing with strongly swirling flow then you are almost certain to be in trouble on the outer wall for the radial velocity component. For the cell next to the wall, you have probably set the "smoothing flux" to zero for the face on the wall but let the large radial pressure gradient create a very large "smoothing flux" on the opposite face. The presence of the large swirl component means the radial pressure gradient is not coupling to the radial velocity component in the "normal" manner. The imbalance in the "smoothing flux" will be creating noticeable accelerations in the relatively weak axial velocity direction via the continuity equation.

I have observed such problems with "Rhie and Chow" pressure smoothing in my own codes and in a leading commercial code. The problem is probably fixable by developing a more sophisticated smoothing scheme but I have not done so nor do I know how to do it. Using grid staggering will avoid the problem.

Actually I am using a staggered grid in order to avoid that problem (I employ the cylindrical coordinate system). Also, the problem does not seem to start on the wall, but in the core flow. I´ve tried to do as you recommended: use a short exit length, let the profiles develop and truncate the backflow. Is there another exit BC I could try?

Thank you,

Francisco.

Evidently this is the continuation of an earlier discussion that I can't locate. Are you in 3-d or 2-d?

If in 2-d, I would assume that it's r-z. If 3-d, meshing the region around the origin (any z, r -> 0) is a nasty little problem as the cells all tend to 3-sided; several vetices merge into the node at the centerline. Can you say a little more about the problem please?

Even in 2-d, the pressure equation must be handled carefully as r -> 0. Since your problem appears to start in that area, you might want to take an extra look at the differencing in the core region.

This is certainly pertinent. I´m working in 3-d and the singularity is treated as suggested by Verzicco and Orlandi (JCP, 123, pp. 402-414, 1996). Honestly, I don´t believe this is the root of the problem, because this methodology has been successfully used for several asymmetric 3D simulations. The problem seems to start in the free vortex region (r> r peak in the tangential velocity), where the axial velocity sign is inverted. Within the region of forced vortex, the axial velocity sign is as expected (upward flow). I must highlight that this does not happen if the upwind scheme is employed (you can see it for yourself in my homepage: www.geocities.com/chicao99br).

Thanks for your remark.

Francisco.

Looks like 0/10 for my first try.

>> Is there another exit BC I could try?

If you are having problems here, there are a lot of variations concerning scaling, truncation, handling the convective component, how to build up the mean profile, etc... which are probably worth exploring first.

Since I am getting your scheme confused with someone elses can you remind us how you solve the set of equations (implicit, semi-implicit, sequential/block).

If you are confident about the centre-line then you must be solving the momentum equations implicitly but this is (probably) not including your convective source terms. These tends to get big in swirling flows making the problem stiff (and you seem to be having problems in the right region for this). One solution to this is to selectively apply more relaxation to these terms (since this is time accurate LES you are going to have do this in an inner loop). Many years ago we used to refer to this as applying "Gosman factors" but I think it was mainly a local term. However, google does throw up one reference to a UMIST report which should explain things better than me banging on here.

For the solution of the governing equations I´m using a fractional step method, with both diffusive and convective terms computed explicitly. For the time advancement, I´m using the 2nd order Adams-Bashforth. For the solution of the Poisson pressure equation, I´m using the BiCGStab. By the way, do you how to impose periodic boundary condtions in the azimuthal coordinate without modifying the linear system solvers?

Regards,

Francisco

>> For the solution of the governing equations I´m using a fractional step method, with both diffusive and convective terms computed explicitly.

No. You cannot do this for cylindrical geometries because you will be violating explicit stability limits in the region of the centre-line for any sensible size of time step. (I believe this is what Jim was referring to above).

I would strongly suggest you add a few lines of code to monitor your convective and diffusive stability limits for every point.

>> By the way, do you how to impose periodic boundary condtions in the azimuthal coordinate without modifying the linear system solvers?

No. You cannot do this because symmetry only exists for the mean flow not the instantaneous flow. You must compute a full 360 degrees if you have a centre line.