Mixing Station with high swirl
Hello to everybody in the forum!
I'm quite new to this and I hope I'll be able to provide some help in future.
But first I've got a problem...
I'm trying to simulate a station for mixing gaseous fuels for the metal industry but I can't obtain a converged solution with a turbulence model different from the standard k-epsilon.
The aim of my simulation is twofold:
a) Calculate the pressure drop between inlet and outlet of the barrel
b) Determine mixing efficiency (as max - min on successive cross-sections on the outflow duct).
Here's the mesh I created using Gambit:
http://img37.imagefra.me/img/img37/2...9m_cfa1987.jpgand this is the mesh on the Outflow duct:
The main gas flows through the the large duct showed on the left of the first image and it mixes with the second flow in the skewed junction. Then they enter the mixer and they are swirled by 12 blades to the external annular chamber, where the third and fourth gases mix with them.
Then they pass to the second section (outlined by the green circumferential line on the barrel) where they pass through a second set of blades, swirling towards the axis and entering the outflow duct with a tangential velocity, completing the mixing process.
I use turbulence and species transport equations (the process is assumed adiabatic).
The mesh obtained for the solid model is good (equiangle skew < 0.86 & aspect ratio < 10.2) and fine enough I hope, but unfortunately I can't obtained a converged solution with the default parameter in Fluent for any turbulence model different from std k-epsilon with a 2nd order of discretization. Anyway I know from literature that k-epsilon performs poorly on such swirled flows.
My boundary conditions are:
- inlets: mass-flow inlet (turbulence=10% and hydraulic diamater);
- outlet: outflow (for better convergence) and at first pressure outlet with/without radial equilibrium pressure option (but I extended the problem domain for avoiding influence of outlet b.c. on the sections of interests, always using std k-epsilon).
I use the following settings:
.Solver: Pressure-based, Steady-state
.Pressure-velocity coupling: SIMPLE
.Spatial discretization: Gradient: Green-Gauss node based
Pressure: Standard / PRESTO! / 2nd order
Momentum, Turbulence, Species: 2nd order
I tried RNG and realizable k-epsilon, k-omega with/without Low-Re corrections and RSM (perhaps the best turbulence model for this situation, because of the high curvature of the flow, as in the case of cyclones) but I can't get a converged solution with the second order of discretization.
Nevertheless I think that this is necessary, because the predicted pressure drop with std k-epsilon is 240 Pa with all discretization at the 1st order and becomes 2400 Pa (a more reasonable value!) with the second order!
Residuals are stuck at too high values (mass 10^-2, turbulence 10^-3) and I often found turbulent viscosity limited and reversed flow at the outlet due to the high swirl.
Here's an example (starting from the solution of a standard k-epsilon at 2nd order):
The situation remains the same even with many other iterations!
In other cases the species residuals at this point begin to oscillate.
Even though I'm not concerned with the outflow, because I extended the problem domain on purpose and this happens only for 1/2 faces on the outflow (as I checked on the axial velocity profiles), I see that other turbulence models are unable to obtain a stable velocity profile on the outflow duct.
The contour plots show waving undefined velocity fields.
I am really confused about the problem...
Is there anyone who could give me some advice, please?
[P.S.: I will partecipate tot the Ansys CAE Conference on the 1st and 2nd of October!]
Use your current solution as a starting point for carrying out an unsteady analysis. Activate the RSM model and switch momentum, turbulence and reynolds stresses to QUICK discretisation. It depends on your inlet velocities and the magnitude of the induced swirl component but stick with the linear pressure strain RSM model initially. You can always switch to the quadratic pressure strain model after you get a converged solution. Mess about with the time step till you get it tuned to your problem, start with something in the range of 0.001 to 0.0001 s. Looking for convergence in about 20 iterations per time step. Your problem is a common one with intense swirling flows and you should notice a pretty fast improvement in your residuals once you switch to the transient solver. Remember to monitor your mass flux error aswell as converged residuals are not the same as a converged solution. Hope this helps you.
Thank you very much, Neil!
I'll put in practice your advices since now and
I'll let you know my improvements in my next posts!
Thank you Neil!!
The improvements on residuals and mass flux error are really impressive using the unsteady solver!
I used 0.0005s as time step and 20 iterations/time step as you indicated and it converges in 5-6 iterations/time step!
This seems quite counterintuitive to me...
Is it only for numerical reasons (but I don't think so...) or is there a physical (i.e. vortex core precessing?) motivation?
With regards to your question, yes it is a physical phenomenon and the steady-state solver is unable to capture this as it is periodic. Usually the steady-state residuals will show massive oscillations displaying limit cycle behaviour as the solver can't resolve the flow properly. A good indication with most problems that you need to do a transient analysis.
If you want to check if there is a PVC look at the tangential velocity profiles which should be reminiscent of the Sullivan vortex model. There should be a relatively linear steep velocity gradient near the axis which indicates solid body rotation and the presence of a forced vortex (PVC). This will be surrounded by the free vortex which relates to the 1/r outer region of the tangential velocity profile. If there is sufficient swirl you should see a low pressure region in the core and get reversed flow, which I expect the solver iteration readouts are saying. Its probably not neccessary but you could define an amination sequence for the locus of zero axial velocity which is the boundary of reversed flow. This is representative of the PVC behaviour because of the quasi-laminar core region causing solid body rotation and will display any precession and deformations of the core. You would likley see the core flapping about near the exit as the circulation strength of the vortex reduces with decay of swirl with length. Confined vortical flows are very complex and intriguing things, if you are interested I would suggest reading sections of 'Theory of concentrated vortices'
Thank you for your interesting reply, Neil!
And for your suggested reading too. I really appreciate this.
Actually, as you wrote, I am obtaining reverse flow warning and the axial velocity profile at the outlet shows a recirculation zone while the tangential velocity profile lays between the profile of the Sullivan vortex (with dv_theta/dr = 0 in r=0, more evidently at the barrel exit) and the profile of the Burgers vortex (with linear distribution near the axis, towards the outlet of the problem domain). This transition of behaviour is probably due to the rapid decay of swirl intensity, I think.
Moreover I have found surprising similarities between my velocity profiles and the ones in a literature case of a cyclone separator for a rotary kiln.
Thank you also for the evocative postprocessing animation that you suggested to me... even though the time interval I simulated is not very long, I am really curious of the results!
Have you any idea for the characteristic frequencies that I have to expect? Or is this a quasiperiodic phenomenon? This case is becoming more and more interesting!
Depends on what frequencies your after. You can easily calculate the PVC frequency from the angular velocity of the core which should scale linearly with inlet velocity. The domain exit is open ended so I wouldn't expect any longitudinal acoustic modes that you can get in helmholtz oscillator cavities. You can always check though by creating a radial rake of points and monitoring pressure over time then doing an FFT on them to see if any characteristic frequencies appear.
The PVC is a periodic phenomenon
That's a very nice tip for postprocessing results!
So I think I will run my simulation with the proper setup in order to:
-obtain an animation sequence for the PVC
-collect pressure and tangential velocity data on two rakes (one at the exit of the barrel, the other in the outlet duct) in order to perform a FFT and compare results with general considerations on PVC that I found on the classic "Swirl Flows" by Gupta, Lilley and Syred.
I hope that the frequency of PVC won't be too small for capturing the oscillations on my simulation time!
Anyway I'm quite new to unsteady analysis and I don't know how I can save time histories from rake points in Fluent for performing a FFT even though I look for a proper procedure in the entire Fluent User's Guide...
You need to go to the solve/monitors/surface menu and pick which positions and what variables you want to monitor, the X axis needs to be set to flow time and have them update with every time step. This will create a .out file which you can then later read into Fluent to do the spectral analysis or change the file extension to .dat if you want to import them into any other software.
The lower the PVC frequncy the better as you don't need smaller time steps then to capture the precession. I don't know what velocities you have calculated but I'm pretty sure your current time step should be more than sufficient.
Thank you very much!!
I will setup my case now, so it will have all the night for running!
Tomorrow I will be in Bergamo for the two days CAE Conference and so I will look at the calculation results only on Monday morning...
Anyway I'll let you know what I will find!
Have a good weekend!
I'm trying to gather more detailed data through time monitoring of pressure, velocities and turbulent kinetic energy in some points of the domain, but now I'm experiencing some problems with the overall mass balance.
This is somewhat related to what you said: residuals go to zero and the solver consider the time step as converged, but the mass flux at the outflow is progressively growing!
Here's what I have on the mass flow rate monitor at the outlet.
The mass flow inlet rates sum up to 39.008 kg/s, so the solution is progressively diverging, I guess.
What's the reason for that? And what are the implicatons on my solution?
Can I control this behaviour only through time step value for integration?
Thanks in advance..!
I doubt the solution is diverging if your residuals converge to the desired limits. I experience this kind of behaviour all the time when simulating swirling flows and unfortunately it is just a case of keep the solution running until there is minimal variation in the mass flux error. From the mass flow plot I can see that there is little oscillation in the mass flow as the solution progresses which is a good thing as it suggests that the time step you employ is suitable. I have run cases before where the mass flow plot has not reached it final value even after 250,000 time steps. You just need to keep going until the mass flow levels out as the flow field you have now can be very different to that of the final solution.
Thank you, Neil... your replies are always very interesting and useful!
Now I'm experiencing what you have predicted about the time step: the oscillations on the mass flow rate at the outlet are getting smoother and even though the value of flow rate at the outlet has reached a minimum at about 38.08 kg/s, now is increasing.
From the other monitors on the rakes of points you suggested me to use I can see that:
- the values of pressures and turbulent kinetic energies are levelling out (the values for k are reaching a minimum in asymptotic fashion all together)
- the values of velocities are still changing as you predicted (some are increasing while others are decreasing).
...So I guess you have great experience on the physics of the phenomenon!
I hope only to have time to obtain a converged solution... my simulation is running since three days! Anyway there's always the weekend!
I will continue with iterations and will let you know for the results!
Have a good weekeend!
(P.S.: I've found another wonderful book... Turbulence in Fluids by M. Lesieur. Really nice!)
As you suggested more than two weeks ago, maybe the latest iterations of the mixing station model show that the convergence difficulties I experienced on the steady state solution were due to the PVC instabilities.
From the first iterations of my unsteady simulation this is my conclusion and I 'd like to know what you think about.
So let's update the convergence history of the unsteday simulation of the mixing station!
First of all, here's the convergence histories plots:
Mass balance history
Axial velocities history (along a and y, two rakes of points respectively at middle and barrel exit sections)
Velocities history in two points of rake y
Pressures histories of three points along rake a
Turbulent kinetic energies histories along points on rake a and y
(and I'm making some animations too! PVC locus, velocities and molar concentrations profiles.)
My conclusions in observing these convergence histories are:
1. The static solution (steady state model) progressively relaxes in a dynamic one (unsteady model) as time advances. Dynamic phenomena of the PVC emerge progressively from the static equilibrium.
2. As a consequence, mass balance is increasingly disturbed and starts oscillating. Hopefully these oscillations should reduce, but the entire process seems to me quite excruciating. Is it possible to speed up convergence without creating instabilities? Mass balance oscillations are to be ascribed to the increasing fluctuations on velocities, I guess.
3. Physical quantities begin to oscillate:
First of all came the velocities, which couldn't be kept at a constant value as they were forced by the PVC, I suppose.
Consequently the periodic variations on velocities profiles induced in-phase oscillations on the pressure values. [Anyway it is possible to see that not all the points in the domain are oscillating in phase and this behaviour seems independent by axial or radial position. The reason for that is not clear for me but I think I'll have to wait for the converged solution.]
Finally the turbulent kinetic energies began to oscillate after a first phase in which they decreased to the same static value for all the different positions observed. What does it mean? I expect them to be static in a RANS approach... or not?
And some other questions on the physics of the observed phenomenon...
How could this be interpreted in the turbulent theory framework? Is that a clue for the isotropy of turbulence (and if so, what about the choice for RSM)?
Can the fluctuations which are now emerging from that isotropic turbulence have a physical meaning? Could this be an indication that RANS cannot capture other dynamics?
Moreover is the sudden decreasing of all turbulent energies an indication for the deviations induced by the k-epsilon model used for the steady state initial solution?
As the solutions converges slowly have a lot of time for these speculations... and so I would like to know what do you think about!
Thank you very much!
First of all the turbulence is not isotropic it is anisotropic. This is why the RSM model is required as the turbulent viscosity parameter of the k-e RNG model treats turbulence as isotropic unlike the RSM model. From looking at the mass flow plot I can see that the oscillations have not settled down into a repeating cycle and the number of time steps is still not enough to get a converged solution. This really depends now on whether or not you want to make a compromise between further CPU time or a relatively converged solution. If the mass flux error and the values of interest are within acceptable limits I would treat the solution as converged. I've seen this behaviour before with the oscillations in various values and it is likely to take a very long time before they dissapear. It is likely that the solver is having problems working out the flow physics and implementation of other models may be needed. Also have you set the backflow species fractions at the outlet correctly?
Further iterations have not settled yet mass flux balance, which appears to be quite erratic...
I am using a simple outflow condition on the domain outlet, which gives me no chance to specify species fractions.
I chose this bondary condition when the first calculations in steady state showed convergence difficulties with a pressure outlet condition with/without radial equilibrium pressure option.
But now I seriously doubt about that...
What should I do in your opinion?
The outflow boundary condition isn't really suitable for this type of simulation and a pressure outlet should be used. If you don't have any idea what the backflow pressure is you could try using a pressure farfield but you will have to extend the outlet boundary to around 5 or 6 times the length of the mixing station. I generally find that pressure farfields also tend to make the solution unstable.
At the moment I would suggest to let the solution run some more and monitor the oscillations and if there is no progress switch to a pressure outlet to see if it has any effect. You could of course just change it now and see if it affects the solution to see if an incorrect boundary condition is the problem.
Ok, so I was totally wrong!
Now that I'm setting the pressure outlet b.c. I have other questions:
1. For the Gauge Pressure I set the same value of Static Pressure obtained though integration on the steady state simulations. It's not that far from the value I can see now on the domain outlet. Is this reasonable?
2. Should I use the Radial equilibrium pressure distribution option?
3. Should I use the Target mass flow rate option to speed up convergence? In this case the choice of the value for the Gauge Pressure shouldn't be so important, because Fluent adjust it until the target mass flow rate is obtained... isn't it?
4. What is the best choice for Turbulence backflow quantities set? K and epsilon / intensity and legth scale / intensity and viscosity ratio / intensity and hydraulic diameter ? Could the same values from the steady state simulations be a nice guess?
I wouldn't use the pressure value from the steady state simulation as the pressure field has not been correctly established and it omits the negative pressure region in the core region. Instead I would use an average value from the transient analysis to set the back flow pressure.
Don't use the radial equilibrium pressure setting because its not true.
Test the target mass flow out as it will adjust the estimated outlet pressure accordingly but disable it is causes divergence.
Use the hydraulic diameter and turbulent intensity at the backflow. Although the Reynolds stresses cause high turbulence production that reduces the rate of turbulent decay and swirl decay, I would use a relatively low turbulent intensity of around 1-3%. You could use values you have already as an estimate but its upto to you.
Now as I checked the turbulence intensities in some time steps I found that the area-weighted average is really high... it oscillates on 150%! The prediction with the k-epsilon was even higher (as you can see from the history of turbulent kinetic energies above).
But if I calculate turbulent intensity as I = (2/3 * k)^0.5 / u_med I find only 10%... This is quite strange to me!
Anyway I'm sorry, but I didn't understand what are your suggestions for the Target mass flow rate option... Could it cause divergence? Or should I use it only for the first iterations just for checking how it modifies the static gauge pressure at the outlet?
Thanks in advance, Neil!
|All times are GMT -4. The time now is 18:48.|