I trying to do that but with not so high pressures at the inlet (around 2e5 Pa, i.e., flow with incipient cavitation). By using the Singhal (or other, e.g. Zwart et al.) model and depending on the turbulence model used, the discharge coefficient obtained is quite reasonable but, pressures along the wall are overpredicted. All papers that I have seen, showed simulations with more high pressures (5e5Pa), with some quite good discharge coefficients results. Nobody modelled cases with less pressure at the inlet. At 5e5Pa there is no data concerning about pressures along the wall, only discharge coefficient is given.
Dear Miguel,
What is the size of the channels you are modeling?
And are you sure that in these low pressures, there is incipient cavitation?
Best,
Morteza
Hi Miguel,
depending to nozzle size your injection pressure will also change. So, it is difficult to say whether this pressure is high or not. For example, we are carrying out experiment using enlarged-nozzle whose thickness and width are 2mm and length is 8 mm. 0.18 MPa corresponds to incipient of cavitation whereas 0.25 and 0.28 are developing and hydraulic flip, which are quite high for this nozzle. Most probably, you should have experimental data of cavitation length and thickness. It is another way to confirm your numerical results. As you said, if the pressure is overestimated along the wall, this means that cavitation underestimated. Than try to play with the model constants to catch reasonable results.
Hope these help.
BR
Baris
Dear Miguel Coussirat,
Since I cannot access complete information of your simulations, I can only give the following suggestions.
(1) When you are using pressure inlet boundary, please make sure that you define a correct static (gauge) pressure and total pressure at the inlet boundary. Sometimes, although you define a correct static gauge pressure at the inlet (e.g 2*10^5 in your case), if you give improper total pressure, it can affect the result. Thus, the total pressure must be suitably given according to estimated flow rate at a particular inlet static (gauge) pressure.
(2) For the simulation of cavitation, the operating pressure and the outlet pressure must be harmonically justified.
(3) Also, the content of non-condensable gas can affect. It is only considered in Singhal model.
(4) According to the information in your comments, I can give these three suggestions. But I am not sure that my suggestions will solve your problem. If you don’t get my suggestions, you may have more questions.
Dear all, I´ll try to give answer for your questions/advices:
I know that Nurick's paper is a bit older paper, but it is interesting because have pressure data at wall. I modelled several cases (Nurick, see paper, Sato and Stutz and Reboud, for Venturis and some others). All cases are for confined flow. For all cases I checked the mesh' sensitivity, using structured and not structured meshes, and also tried with adaptative meshes. One of the goals for me is to know the minimal cells quantity, in order to obtain good results because after, I'll use the cavitation model in turbomachinery problems....
Dear Morteza/Baris, in the paper you can see in table , the geometry. I tried with the lucite device geometry, in spite that there is flipping flow, when the pressure drop is increased, because many people use it for CFD testing, but with a pressure of 5e5Pa. Them say that cavitation is a pressure leaded phenomenon, then it is not necessary to define so much cells,... (I'm not agree with them). Also, for low pressures there is a graphic where measured pressures in two places (figure 5), related with the inlet pressure, are shown. Here, you can see that pressure falls until vapor pressure in the two sensors for a pressure value of 1.85e5 defined at the inlet .
Dear Baris, I tried with several geometies (i.e. Venturis, see papers from Stutz and Reboud for steady and unsteady cavitation). In this case I obtained similar results as Gonçalvez et al for velocities and vapour fraction into the cavity, not so good but not so bad.... But in Nurick's case, I cannot obtain good pressure values at the wall. Was a suprise for me.
Dear Nay. Yes, I check it. I use the total pressure (absolute) and I put an initial/gauge value in order to obtain a suitable velocity value for initialization.
I defined the operating pressure at the outlet (95000Pa, atmospheric pressure as experiments say), and define outlet pressure as a pressure gauge respect to the operating pressure.
And also I try with several values for non-condensed gases. I also used others cavitation models available in Ansys Fluent but I obtained similar results.
My conclusion at the moment is that when I have sudden contraction the separation is more stronger than in venturis and the values for velocities are not well defined at the wall (I checked with two layer modeling also,... similar results...). May be it is neccesary to use a very refined mesh (I tried with 250.000 cells 2D axisymmetric problem, I also check 3D geometry... similar results).
May be I'll can write a paper with my no-results... :-)
Thanks to all!
Miguel
Dear Nay!
No, don't worry!. I only try to expose my arguments in order to make a clear answer to your questions/advices. Really it is very interesting give answers and arguments of my work to other people. It is not easy to discuss these topics in non-conference forums.
Best regards!
Miguel
Dear Hamed,
I have red carefully your work. It is very interesting and, you can help me if you check my comments about your work. I know that my speech is a bit large, but I think that is very interesting to interchange opinions about this. Best regards,
Miguel
--------------------------------------------------------------------------------------
1. Digitalized data from Nurick shows that saturation pressure is a bit over 3400 Pa. But I, recognize that the error in measurements were not given by Nurick. In agremeent with you I have a value of 3540 Pa.
2. The Nurick data did not show temperature of the experiments, therefore I took the temperature of saturation that agrees with saturation pressure from experiments.
3. This temperature was 27C, therefore, in my opinion, the dynamic viscosity for the vapor that you are using is wrong(you have 1.26e-6 kg/m s) . I think that If you have a density of 1000kg/m3 in liquid phase, you cannot have the vapor phase viscosity that you used in your paper. Isn't?. The value from tables is 9.9241411770818E-6 kg/m s. I recognize that when a `mean´ value of viscosity is computed (when the `mixture' viscosity and density, are computed by a CFD model), would be not very affected for the difference.
4. I only defined a suitable inlet pressure, in order to obtain a sigma value between 1,75
Can anyone let me know what was the cavitation number range for above study??
Dear Sachin,
Check some of my publications in this Website. The last one is from 2017 There is other in the JFE Journal. You can find it in the "cloud" using my lastname, turbulence and cavitation keywords... Best regards...
- Badges
- Science topic