problem with turbulent model in free surface
 

I use k-e and RNGk-e for my free surface flow model, but the result of k-e is better than RNGk-e is the possible? because most papers said RNGk-e is more accurate than k-e in swirl and high curvature flow.
the second question how can I calculate Fr (v/(g y)^0.5) in CFX post in a section where v is the average velocity and y average hight at that section.
thanks:

please can anyone help me in that problem

There is not much difference between k-e and RNG k-e for most applications. And I would expect them to both have similar problems with swirl and high curvature flow - you need RSM models to handle that.

The equation you quote should be easy enough to process in CFD-Post. What is your problem with it?

well, first thanks for your reply
the problem in that equation is, how can I express average velocity for example at plane 1, is that right (avgvelocity@plane1) or something like this
about y or height of water, how can I express y at VF 0.5. this is my problem.
thanks

If you have a plane, then the areaInt(water.vf)@plane/area()@plane is the proportion of the plane which has water. There's a starting point for you.

thanks
about turbulent model, I think your purpose is, in spite higher computational time of RNGk-e it is result almost similar to k-e, so which kind of turbulent model of Reynolds stress model (RSM) is useful to handle that case, (LRR Reynolds Stress, QI Reynolds Stress, SSG Reynolds Stress, Omega Reynolds Stress, Baseline (BSL) Reynolds Stress model, Explicit Algebraic Reynolds Stress model)
are available in CFX

?????????????

I do not understand your question.

Are you asking what turbulence models are available in CFX? (the answer is: it is all in the documentation, read it)

Or are you asking what turbulence model do you recommend for your application? (the answer is: I always recommend using SST unless you have a good reason not to. You have not stated a good reason not to, so I recommend SST)

of sure I know the turbulence models that available in CFX
yes, my question about best turbulence model for swirling and high curvature flow like hydraulic jump.
but I think SST at the same class like RNGk-e, standard k-e (which is eddy viscosity model), I test RNGk-e, standard k-e almost have the same result.
according to your previous post that RSM is the best to handle that high flow curvature, my question is what specific model in RSM in CFX there are many model as I posted previously.

No, I do not agree. The curvature I see in the hydraulic jumps I am familiar with is more a turbulent effect, that is it is random in space and time. You do not need things like RSM models to handle this a standard model like SST should work. Well, at least I would try SST first.

The flows which definitely have high curvature which mean 2-equation models like SST are unsuitable (at least without modification for the curvature) are things like industrial cyclone flows. The streamlines have extreme accelerations on them in this case.

But at the end of the day if you get good results with RSM and poor results with a 2-equation model then that is convincing to me.

I tested SST but its result is like k-e in hydraulic jump, what is your suggest

You suggested RSM models. Have you tried that?

no, because there are many models corresponding RSM, which model is the best, because I can not test all models due to high computational time (my model is big)

All the models have strengths and weaknesses, so none of them are "the best". If you read the documentation the SSG RSM model is probably the one to try. If want to try a omega based model try BSL RSM.

I used RSM but its result similar to other turbulent models
at the end of channel there is 8 cm difference with experiment, which is very high, I dont know why. is it possible to say CFX (RANS, with turbulent model) does not work in hydraulic jump.
my mesh and all BC are correct only Iam not sure about outlet B.C
I used outlet BC at the end of channel (at drop) with super critical, and at bottom of channel with static pressure = 0

https://drive.google.com/open?id=0B3...0h4VzBLUGJEVlk
https://drive.google.com/open?id=0B3...kM3T3QzZUdqaWs
https://drive.google.com/open?id=0B3...EtpVWZseGVTdUE

CFX can model hydraulic jump. You have not set it up correctly. But the hard bit is finding what you have done wrong.

These results also suggests the turbulence model is not causing the problem, as you say the problem is more likely in you fundamental simulation setup.

From your images I can see lots of problems straight away:
* Your mesh is way too coarse
* Your inlet is too close
* Your outlet is too close

So they are some things you need to fix before you look at anything else.

thanks, sorry the above attached image is only a part of my model (only jump location) see bellow, , as you said your mesh coarse, I think only due to there is no sharp inter phase between air and water, is that?? (this is very common because water mixed with air so sharp interphase very hard to obtained even if very fine mesh selected), my inlet is far from jump and outlet by about 0.8m (at location of drop, so I can not put it further upstream), at this condition what is your suggestion

https://drive.google.com/open?id=0Bz...DhVYTNjLWZLVnc

Regarding the coarse mesh issue, have you attempted to run a finer mesh and see if the solution is sensitive to the mesh resolution ?

The use of coarse, medium, fine, etc meshes is just relative terminology for a given problem. What is coarse for a case may be just fine for another regime ? There is no generality, and sensitivity studies must always be done to some extent.

good idea

of sure first I did sensitivity analysis for mesh size and turbulence models, for mesh three mesh count (1.3 million, 2.5 million, 3.8 million) selected, the result of medium and fine mesh very close, for turbulent models (k-e, SST, RSM) can not predict actual free surface at jump location, but at other location where air doesnot mixed with water there results are good agree with experiment.