Learning Forum

[vangelis]

Hello to everyone,

for my diploma thesis I am required to develop a flow field for a 2D Francis turbine. For this model the overset technic is implemented for the runner. The problem is that turbulent viscosity ratio problem and generally high turbulent viscosity ratios are developing if a choose a time step larger than about 6e-05 sec or about 0.07 degrees of rotation (the turbine is operating at 333 RPM). Although incredibly time consuming, I have been forced to choose this time step, but still another problem arises. Reversed flow at the pressure outlet is oscillating between 50 to 60 faces out of roughly 200 outlet faces.

Not much can altered in the boundary conditions, at least regarding thy type of the boundaries, due to compatibility issued with the overset technic. The same applies with solver type, scheme types etc.

I know this problem can be solved because I have a solved and converged Ansys fluent similar case in my hands, so it is actually a matter of proper initialization and proper early simulation runs. Probably there are some technics but I am not aware of them. 

Bellow I am attaching some screenshots of the problems I mentioned to see for yourselves,

Thank you.
My turbulent viscosity ratio contour plot:

What happens if I increase the time step one order:


Cells between 50K and 100K (with the lower time step none cell is above 40K):


Reverse flow problem:


With velocity vectors:



Velocities make no sense if I increase the time step one order of magnitude:



I am reminding the time step is 6e-05, and the increased time step is 6e-04 sec.

Here is how the similar case I have in my hands residuals look like:



In only 1 sec flow time solution is fully converged, no problems and pretty robust, as it works fine with quite large time steps (6e-03 for example). I am not attaching the contour plots for this case as they look completely normal, with no errors. Perhaps some expert can identify the initialization technics used by the residual monitor plot.

Thank you for your time in advance.

 

[jabanto]

Hello Vangelis

Thanks for posting the question and for sharing the images.

It is not clear from the description and images what type of settings you have in your overset case. Is this a transient MRF? or sliding mesh? or dynamic mesh with prescribed rotation? Or, a 1dof rotation? How many orphans you got in your overset mesh? Is it increasing during simulation?

Here are my comments and/or recommendations:

0) We assume your mesh is ok, with a minimal (or 0) orphans, with good mesh resolution and distribution, good quality metrics (skewness < 0.9) and y+ ~ 1 if you plan to get accurate results. We assume the (cell/boundary) conditions applied are correct as well as the time step size.

1) You may not need overset to resolve this problem. But, if it is required in your thesis, please plan running your case also on regular (non-overset) mesh, this will help you with the conclusions in your investigation. Overset is a non-conservative method, you should expect some differences compared to the results from non-overset runs, but the differences shouldn't be large.

2) Realizable k-epsilon is a good option. Consider SSTkomega.

3) If you are using MRF or Mesh Motion (sliding mesh), initialize the flow 'absolute' frame (not from 'relative' frame, default). 

4) Start a transient simulation from a well converged steady state MRF results.

5) Such geometries have gaps between the blade tips and the volute. Use boundary distance donor priority method.

6) You may need to consider ideal gas or compressible liquid, accordingly.

 

Not sure if this will help, but I just wanted to post these comments only.

Best regards

Juan Abanto

 

 

[vangelis]

Dear Juan Abanto,

thank you very much for your response, spending your valued time to reply means a lot to me. Sorry for late reply but I was really consumed with my subject.

1) Mesh is OK with no orphan cells and mesh quality is good. However, I have not yet checked the y+ value I will do though.

2) overset mesh is compulsory for my thesis

3) I have recently read tha the k-ε model is prone to turbulent viscosity issues, meaning it produces non-real results when using multiple reference frames and rotating domains. Sadly, I have experienced this issue because obviously, a water turbine has a rotating domain. In particular turbulent viscosity ratio is skyrocketing near the border of the rotating and stationary domain and slowly spreads through the entiry mesh domain.
This is happening everytime unless extremely low time step is used which is obviously both time and resource consuming.

4) I am already doing this

5) Yes, but I have no gaps because the turbine runner is also modeled through overset  technique, I don't have guide vanes or any other adjustable vanes. Only the runner.

6) The truth is that I have not considered that, but I thing the problem lies in number 2 point.

Last about number 2, I have also read that the best model for near wall treatments, and generally flows that are very close to wall are the k-omega models... so I tried a k-omega simple model and the results were good, no errors, but vastly different from the k-epsilon model especially in terms of turbulent viscosity
I will also try the k-omega SST model, which I read that it practically switches between the k-epsilon and k-omega automatically to provide the best model for any occasion.
Also I am particularly interested about near wall flows because I am simulating the movement of a small object inside the water turbine, testing for its trajectory and any possible collisions. The reason I have not yet tried another turbulence model was that the phd student that is assigned to supervise and help me strongly insisted on using the k-e model.... not having any knowledge on the subject I listened to him

Now having read all that about k-e and k-omega models, and also reading the same suggestions from you means a lot and I am confident to move to this direction.

Thank you again, I will update soon.

[vangelis]

 

0) We assume your mesh is ok, with a minimal (or 0) orphans, with good mesh resolution and distribution, good quality metrics (skewness < 0.9) and y+ ~ 1 if you plan to get accurate results. We assume the (cell/boundary) conditions applied are correct as well as the time step size.

 

 

Y plus is about 9 on the casing wall and about 15-16 on the runner blades. This with the k-epsilon model, is the another indication that I need to change the viscous model to k-omega or k-omega SST?