I'm running a 2D axisymetric simulation with swirl. The swirl velocity is very high and I have a problem with backflows in the pressure outlets. During startup of my case it is almost impossible to avoid getting backflow in some of the pressure outlets. When this happens the flow coming in will have zero swirl velocity and this will create all kinds of problems because the surrounding fluid has a very high swirl - the turbulence model explodes and you get a pocket of "non-swirling honey backflow" that never dissapears.

One solution could be to be able to somehow specify the swirl in the backflow, like you can specify k and epsilon etc. in the backflow. I don't think this can be done in Fluent though, unless perhaps with a UDF. A nice solution could be if Fluent automatically as default would set the backflow swirl to say the average swirl of the outflow part of the outlet.

Has anyone got any better suggestions on how to solve this problem? Perhaps someone has written a UDF for something similar?

set a bigger gage pressure value for the pressure outlet, after a certain iterations set it back to your real gage pressure. It may works. Tudi

Eh, I don't see how that could improve the cituation. Rising the gauge pressure will just give you even more backflow and thus more problems with the differences in swirl velocity between this backflow and the fluid in the domain.

I've tried the other way around though - reducing the gauge pressure and thereby "suck out" the problems. This doesn't help once the problems have occured. However, if you combine this with an intelligent patching (based on turbulence intensity and swirl level) of the swirl field and k field, then it seem to help. But then when you start rising the gauge pressure you will run into the same problem again - as soon as you get just a little bit of backflow in one single cell the swirl-difference makes the turbulence explode.

Are both the physics and geometry of your problem axisymmetric? I use swirl to minimize wall separation. At times your flow can seperate from some part of your domain and it is attached on some other parts. This can happen even when your geometry looks perfectly axisymmetric.Thus it is possible that you are using an axisymmetric model for a truely 3-D problem. In such cases you will have a lot of 'blow ups' and convergence problems.

Is your flow compressible or not? Is it subsonic or supersonic or both? These are important to know since boundary conditions for these kinds of flows are sometimes treated differently from their incompressible counterparts.

Thanks for your answer. I agree with you that in reality many swirling flows are 3D and unsteady. However, the problem I have here is more fundamental - it is localized to the pressure outlets and it is not a general stability problem associated with the strong swirl or so.

To answer your questions. The geometry is axisymmetric in my model, the real case is not completely axisymmetric though, it has a few small non-axisymmetric details. The flow is mildly compressible - mach numbers below 0.7 everywhere and below 0.2 in most regions. I use the segregated solver with viscous heating and ideal gas. I also use the PRESTO scheme for the pressure (improves things significantly).

Jonas,

I'm alsmost sure that you've tried all these. But ...

Doesn't "Radial Equilibrium Pressure Distribution" option help ? As you know, this option accounts for the fact that there's a radial pressure gradient when the flow is swirling. This option has often been found to reduce or suppress the backflow.

And one more thing. If the flow is entrained into the domain through pressure outlets, it's recommended that freestream turbulence quantities are set on pressure outlet boundaries. The defaul (k=1.0, epsilon=1.0 in whatever units you're using) often cause problems in terms of convergence and yield unphysical results.

Yep, I use radial equilibrium on the outlets. I've also tried changing the backflow k and epsilon settings. This doesn't help either - the problem is the strong shear produced when non-swirling backflow meets the strongly swirling flow in the domain. Couldn't you you implement a backflow swirl paramater for the pressure outlet boundary condition when used with swirling flows?

For time dependent calculations, try fixing the UR (under-relaxation factors) and starting with a very small time step (like 0.0001 secs). Increase time step gradually (leaving UR fixed) as flow stabilizes.

For steady flow, start with low UR values, like 0.000X for pressure (continuity), momentum and energy with turbulence turned off. Gradually increase these values simultaneously. When 'good behavior' is realized in your flow in your domain, turn on turbulence with UR values as low as you started the laminar flow with. Gradually increase to quickly get to steady state. You tell me what good behavior means. Good luck.

I'll try this approach tomorrow. Thanks! I think that the key to success is to find a way to avoid ever getting any backflow on the problematic pressure outlets. I might have to extend them a bit also in order to move them further away from recirculation zones etc.

Have you ever observed any similar problems with non-swirling backflow from pressure outlets into swirling flows causing "exploding" turbulence?

Pressure outlet is sort of a entrainment boundary. My concern is whether you'll be able to specify "backflow" swirl with reasonable confidence that it actually represents the reality.

You can adjust the swirl velocity at inlet and outlet boundaries using UDF(DEFINE_ADJUST). In fact, you can adjust any solution variables on boundaries using the DEFINE_ADJUST. But frankly, I don't clearly see what we want to achive by doing that.

Sung-Eun, thanks for your help. Reasonable confidence or not, something which is close to the swirl of the main flow will be better than zero, as it is in Fluent today. Surely, in my case, zero swirl in the backflow is very bad, much worse than a roughly estimated mean swirl. In my particular case the outlets are "rotating holes" modeled axisymmetrically as an ordinary outlet, hence it is quite easy to estimate the backflow swirl since the rotational velocity of the "holes" is known.

I don't see any principal difference between specifying a backflow k and specifying a backflow swirl. Is there?

I'll look into the DEFINE_ADJUST trick. Thanks!

I've looked a bit at the DEFINE_ADJUST function. I understand how this function can be used to adjust a solution variable in the whole domain, but in my case I'd like to only adjust the swirl in the backflow regions of pressure outlets, preferably independantly for each outlet. Is it possible to do that?

I couldn't find any examples where DEFINE_ADJUST was used only to modify a specific boundary condition. If anyone has any examples of that I'd be very greatful.

(1). The problem you are trying to solve is a real problem. (2). But in order to have a solution to the type of problem, that is a turbulent high swirl flow with possible flow separation at outlet, there are several factors have to be considered first. (3). For the turbulence modelling, the consistent wall treatment has to be enforced. And when the wall shear stress goes to zero, a lot of things can happen there. Mathematically, one needs to work out every possibilities. (4). In many cases, the equations of the turbulence model are solved separately, that is outside the main loop of the momentum equations. The way they are solved and the solution sensitivity to the boundary conditions can affect the convergence of the solution. (5). Then back to the main loop solution algorithm, whether the boundary conditions are sufficient and consistent to provide a converged solution itself is a big question. I can't go too deep into this issue, but you sure can run some exercises to find out. (6). When you say "backflows in the pressure outlet", I think, you are talking about "partial reverse flow at the outlet". That is a portion of the flow is moving out, and portion of it is moving into the computational domain at the outflow boundary. You need to verify first that such condition can exist in the formulation you are using. I mean, will it come to a stable location such that partial reverse flow exists by using the options in the code. (7). I think, most commercial codes provide only simple inlet, outlet conditions which exist in simple flow problems with simple inlet and simple outlet flow conditions. (8). For more complicated flow problems, these simple inlet and outlet conditions may not be consistent or adequate for a solution at all.

You have understood my problem correctly - it is a partial backflow in a region of the outlet. I do get a stabilized solution, but it is not physical (extreme shear due to the lack of swirl in the backflow which gives exploding turbulence in this region). The solution in the backflow regions also is unsensitive to the outlet pressure - I can set it to vacuum and still not get rid of the backflow in these regions once it has occured. Hence, the solution is not physical.

I think that the implementation of "backflow" in pressure outlets in Fluent should include a parameter for the swirl also, or what do you think? Today you only give k, epsilon and total pressure.

(1). There are a couple of solutions to this particular problem. (2). Since the reverse flow region is relatively stable, and you are getting zero swirl from the downstream side, you can specify the reverse flow potion as a wall boundary condition. (3). The artificial wall will stop the reverse flow and also the influence from the downstream condition. This should be easier to do. (4). The recirculation buble should still be there, I hope. (5). The other approach is to create a second inlet there. Instead of a wall, now you have a second inlet, I mean artificial inlet. (6). With this inlet, you can specify the usual inlet conditions there to study the flow behavior.(to cover the reversed flow portion of the outlet, assuming that you have done the first run.) If it is necessary, you can put a small divider wall between the official outlet and the second artificial inlet. ( Although I am not currently using the code, I had modelled a problem with several inlets, so I think, you should be able to do it with the code.) The need to use a divider wall is just a guess, to avoid complication due to over-simplification. (7). The use of a wall or a secondary inlet is just simulation techniques only for advanced users. In this way, you can choose not-to-specify or to-specify the reverse-flow portion of the outlet.

I haven't read all of the responses to the question, but I'll throw in my two cents anyway.

Flows with swirl numbers (the swirl number is typically defined as the ratio of the tangential momentum flux to the axial momentum flux) larger than about 0.6 will develop a recirculating flow pattern when it goes through an expansion. The book "Combustion Aerodynamics" by Beer and Chigier discusses this in the context of stabilizing a combustor. That book is out of print. For combustors, the recirculation you are observing is used to bring hot products of combustion back to the reactants and ignite them, leading to a stable flame.

My point here is that your boundary condition location may be leading to a poorly posed problem. I wish I could draw you a sketch to better explain my point. I would suggest moving your boundary condition further downstream. In the sort of flow I am describing, there are two stagnation points on the axis, one near the expansion where the recirculating flow meets the main flow, and one downstream where the recirculation ends. If you move your boundary downstream, then plot axial velocity on the axis you should be able to find these stagnation points.

Of course, I may be dead wrong about your problem!!

I have problem with the backflow at pressure outlet almost at every calculation of turbine runner operating at off-design conditions. Simple back flow at pressure outlet can be found also in case of swirl flow at straight conical diffusers. The problem is as you described that the back flow is entering the domain with zero swirl velocity. The problem of this kind of back flow is physically in correct and can be also experimentally confirmed. But, the tangential velocities are not zero at experiments. The solution how to solve this problem in Fluent is only one, I think. Try to extend the domain and move the outlet boundary condition downstream from the back flow zone. I do not know your problem but the good solution could also be to use the extension to the large outlet tank.

I carry out the rotating periodicity calculation with the rotating periodicity and with the mixing planes. The back flow zone at the pressure outlet condition (upstream b.c.) at this mixing plane was found. The tangential velocity components were found to be zero at this backflow zone region. On the downstream side of the mixing plane (at pressure inlet b.c.) the tangential velocity components are not zero even in the backflow zone. Does it mean that there is no continuity between tangential velocity components at the mixing plane? Can you advice how to solve the problem with the back flow at mixing plane?