[Dranzer]

I am new to CFD, I am working on mixing in Stirred Tank. I am facing problems in mixing profile. I am using MRF, while simulating it seems to me that the fluid inside the rotating domain is rotating properly but the velocity is not imparted outside the impeller. The velocity fades just near the interface and even in the vertical direction the velocity is fading very fast. The mixing profile is not coming out to be proper.
I am using Standard k-epsilon with standard wall functions, Explicit Euler.

[CeesH]

hi,

1) if you check your boundary conditions, are you sure there is an interface between the 2 zones in your tank (and not a wall or so)

2) how many iterations did you do? are you sure the simulation is done? In my experience, during iterations the velocity profile is calculated pseudo-transient: first things around the impeller start to move, then the rest of the fluid. Cut of too early and it seems like there is motion in only 1 frame.

[Dranzer]

Hi
I myself assigned the boundary conditions to be interface and defined mesh interace. I was going to do the simulation in two stages, one for steady state without air and after that the transient simulation. But in the steady state the iter for v-air was not converging so have to increase the convergence criterion for that so having the simulation done in lesser iterations.

[CeesH]

Ah, you are doing 2-phase? That makes life somewhat more difficult.

Could you provide the results (contour plot + mesh) of a single phase simulation, in steady state?

Best,
Cees

[Dranzer]

Hi Cees,
Please find attach the velocity vectors on a x-plane and a y-plane.

Regarding the wall thing you said earlier, I noticed that whenever I define a mesh interface Fluent creates a wall zone for each interface zone as a Boundary wall. Does this affect the calculation?

[CeesH]

I think that interface definition might be the problem indeed. As long as you do not have any periodic boundary conditions and are not using sliding mesh, you don't need to define any special conditions on the interface - just matching them is sufficient.

[ghost82]

Originally Posted by Dranzer

Regarding the wall thing you said earlier, I noticed that whenever I define a mesh interface Fluent creates a wall zone for each interface zone as a Boundary wall. Does this affect the calculation?

It depends (if your 2 surfaces which define the interface are 100% overlapping it's ok): an interface is made of 2 surfaces: not always the 2 surfaces are 100% overlapping.
Everytime you create an interface fluent automatically creates a new wall zone, which by default is a wall defining the non overlapping surface.
Try to plot this new created wall surface: if nothing is shown in the graphic window then it's ok.

[Dranzer]

Originally Posted by ghost82

Try to plot this new created wall surface: if nothing is shown in the graphic window then it's ok.

Plotting as in checking the mesh. If I check the mesh for the face, I get nothing. So from what i was able to comprehend, the wall is not a problem. If I am right then what can I do to fix the problem of the velocity profile.

[Dranzer]

Help Please
I earlier posted the velocity vectors for single phase simulation in a stirred tank reactor in Rushton Turbine. The velocity is not being properly transferred outside the interface.I am not able to troubleshoot it.

[CeesH]

For the vector plots above (these are steady, single phase right?), how many iterations did you do and what did you base convergence on?

Best,
Cees

[Dranzer]

Yes, they are for single phase using water. I took a criterion of 0.001 for residuals. It took me around 600 iterations.
Thanks in advance

[CeesH]

Try 10^-5 and a lot more iterations. My experience is that a stirred tank takes 2000 - 15000 iterations to converge, depeniding on mesh quality and so on. Also put on some monitors (mean velocity magnitude, moment coefficients) and see whether they converge to a constant value. Judging convergence on the residuals alone is not good practice!

Due to the way the problem is set up, the velocity profile will first develop around the impeller and then further develop into the rest of the domain; in that sense it looks as if the solver works pseudo-transient (even if you do not tick that option!). If you stop the solution process too early, it may look as if only the rotating domain is solved. This is not true, the simulation simple hasn't finished.

[Dranzer]

Dear Cees,
Your idea of more iterations satisfactory results but my solution is not staying stable for such number of iterations.
So what should be the approach to solve Stirred tank like combination of urf and solution methods?

[CeesH]

How big are the oscillations you are observing? Are the residuals also 'stable' (that is, oscillating but not going down on average)?

I would take second order upwind for all flow variables, standard pressure scheme and a URF of 0.1 - 0.2 for momentum.

If that doesn't work, check if you can improve the mesh.

Best,
Cees

[Dranzer]

I am not able to get residuals below 5*10^-3. After that it becomes unstable. Can you tell me how to get higher quality mesh. I am using automatic settings of the ansys meshing software

[CeesH]

but what are your levels of mean velocity fluctuation at that value of the residuals?

For a stirred tank, assuming you have rushton turbines, you can make a structured hexagonal mesh. If you have another type of impeller this is difficult in ANSYS mesher, but you can easily make a non-structured mesh around the impeller and a structured mesh in the bulk

[Dranzer]

Hey can you explain how can I check the mean velocity fluctuations? I am checking convergence only through residuals.
Also in my case the skewness of some of cells goes around 1.00, even I tried to increase the relevance(for hexagonal mesh) but of no use. Can you tell me any resource where I can generate less dense high quality mesh.
P.S. Till now I am using Ansys Mesher

[CeesH]

Checking converence by the residuals alone is bad practice - it only indicates your solution is getting better with respect to the initial guess (or, in case the residuals go up, it's getting worse), but it does not say anything about how good the solution is in absolute terms.

So, if you make a monitor for volume-average velocity over the number of iterations, how big are the fluctuations that you observe? If the mean is, say, 1 m/s; do you see oscillations between 0.9 and 1.1 (which would be problematic) or maybe between 0.995 and 1.005 (which would be much more acceptable).

Regarding the mesh: if you use a rushton, you can make 0-thickness surfaces out of the baffle and impeller rather than volumetric objects, and this allows you to use sweep hex-meshing.