Transient cavitating flow around a stationary hydrofoil
i have already performed a transient simulation of the cavitating flow around a stationary hydrofoil (e.g. CFX Tutorial Chapt. 21 "Cavitation Around a Hydrofoil") using kOmega SST turbulence modeling and the "standard" Rayleigh-Plesset Cavitationmodel which is already implemented in CFX.
Now, i have some futher questions regarding this matter. The most important question is about managing the result-data in CFX Post:
1. Does anybody know if CFX uses the Kubota model for calculating the masstransfer rate between liquid and vapor phases during cavitaion ??
Few cavitation models are available. For example: Merkle, Singhal and a few more. Comparing the CFX masstransfer equations for cavitation modeling to literature references, it seems that CFX uses the Kubota model.
Does anybody agree??
2. Does anybody has any experiences regarding the implementation of user defined cavitation models ?
3. i want to obtain the drag and lift coefficients as a function of time (transient run) in a chart (Post):
thereby, i used the following user defined expressions for c_lift and c_drag:
and ...force_x()... for the drag coefficient.
Does anybody agree with this procedure?
4. does the force_() function in Post consider both the pressure and the friction forces?
And does the function already considers forces due to both phases ocuring during the cavitiaon process?
The results show cleary the frequent shedding of cloud cavitation vortices. I want to visualize both the drag and the lift coefficient on the hydrofoil as a function of time. The aim is to obtain the frequency of cloud cavitation vortices. Therefore i want to use the FFT analyse function in CFX Post. Calculating the shedding frequency with FFT is only possible if c_lift behaves like a periodic oszillation?
I would be very helpful for further help in this matter!!
I have little experience with using non-default options for cavitation so cannot answer your questions on other cavitation and mass transfer models. Your questions about what does CFX use are answered in the CFX documentation.
Your CL and CD equations appear to use areaAve(Density)@Profil - this will take the average density over the foil which might include some cavitation regions. Usually the reference density is taken as the free stream liquid density. Also area()@Profil will give the total area of the foil, whereas you probably want the area projected in the y direction (ie planform area).
4. Both pressure and viscous components - yes. Both phases - yes.
Thanks for the reply!
you are right, using the areaAve function at the Profil is not meaningful. i made a mistake. The function should be like: areaAve(Density)@Inlet.
Usualy, the formulation for the drag and the lift coefficient both take into account the entire area (=length*hight) of the wing. anywhere, is there another function in post available instead of "area". i.e. for a planform area as a projection in x or y axis direction ??
Be careful with areaAve(Density)@Inlet as well! If your inlet has both water and gas phases going through it then it will return a strange number. Just set it to the density of the liquid phase.
Assuming the surface Profil is the entire foil (ie top and bottom faces) then area()@Profil will return approximately 2*length*height as it includes top and bottom faces. Have a look in the CFX Reference manual for available functions.
When you are developing CEL expressions it is a really good idea to use a monitor point to output the CEL expression value. Then you can check it doing what you expect, and you would catch the unusual gotchas I am talking about.
hi Kimotbwb, i want to take a transient simulation of the cavitation flow in a centrifugal pump ,but i am not sure how to handle file the set in the transient simulation pre, so can you give me some suggestion?
I'm looking forward to you reply！
thank you !!
|All times are GMT -4. The time now is 17:28.|