[dinhanh]

Hi, I am new in CFD
Now I am doing cavitation transient calculation inside a nozzle for my thesis. I read in the fluent user guid that, the residual should be reduce 2 or 3 order. But I do not really understand that.
This is residual plot from my calculation. Could you tell me how good this residual is?
Thank you very much!

[dinhanh]

For more information, in the monitor residual panel, I turn off the crition check. Is it OK?

[pakk]

Originally Posted by dinhanh

I read in the fluent user guid that, the residual should be reduce 2 or 3 order.

That means that if the residual starts at 1, it should be reduced by a factor of at least 100 or 1000, so it should be lower than 0.01, preferably lower than 0.001. (100=10^2, 1000=10^3, that is what the order 2 or 3 means.)

Your continuity (white line) goes from 0.008 to 0.0008, so that is a factor 10. I don't know what happened before iteration 1500, but if you really started at iteration 1500, I would say this is poor convergence.

[dinhanh]

Thank your quik answe,

I did steady calculation for single phase for first 1500 inter. after that change to unsteady and cavitation model. As you sad, continuity residual is poor. How to improve the convergen?

Ps: Also, I get message:"reversed flow at xxx face on pressure-outlet". So it may cause that problem to poor convergence

[ghost82]

Usually for cavitation simulations time step should be very small: I usually set a maximum time step of 1e-5 down to 1e-7.
Extend your domain at the outlet, plot contour to see what is causing reverse flow.

[dinhanh]

Originally Posted by ghost82

Usually for cavitation simulations time step should be very small: I usually set a maximum time step of 1e-5 down to 1e-7.
Extend your domain at the outlet, plot contour to see what is causing reverse flow.

Thank ghost82,
Extend the domain may be effect to the solution? Because in the nozzle flow, pressure fall down to saturation pressure and increase to reach pressure at outlet. So I think if domain extended, then pressure will be slowly to reach outlet pressure, and the aspect of cavity will be different.

[ghost82]

I think no, not so much..if you extend, for example, the outlet 10 cm far, you have only more pressure drop due to 10 cm pipe (which are negligible). You can always subtract this pressure drop at the "new" outlet.
I think it will not affect the cavity length.

[dinhanh]

Uhm, I see. You are right. And how about the residual? How to improve tohave the good convergency. I dont think have any problem to grid. The grid is structure and I checked: othogonal, skewness, aspect ratio which are good.

[ghost82]

Originally Posted by dinhanh

And how about the residual? How to improve tohave the good convergency.

Cavitation problems are transient problems: simulating steady state solution in most cases is not the right choice. So first thing is to switch to transient solver (and you have already done it).
It seems you have no problems in residual behaviour: I think that lowering the time step and adding some more iterations per time step (like 40-50) should do the trick.

[dinhanh]

Thank you for your comment, ghost82!

[dinhanh]

Originally Posted by ghost82

Cavitation problems are transient problems: simulating steady state solution in most cases is not the right choice. So first thing is to switch to transient solver (and you have already done it).
It seems you have no problems in residual behaviour: I think that lowering the time step and adding some more iterations per time step (like 40-50) should do the trick.

Hi, ghost82
I extended the domain and reduced the timestep and also increased interation per timestep. The message: "the reserved flow at XXX face on pressure outlet" gone. And I think I got better residual. I upload the picture about new timestep and residual as below.
How do you think about this?

[ghost82]

Hi, I think it's ok.

[Kozan]

Hello,

Have you succeeded with your simulation? I'm solving cavitation in the nozzle with circular cross section, using 2D axisymmetric solver, RSM model of turbulence and Schneer-Sauer model of cavitation (Ansys Fluent 15). I did simulations of 5 operating points until now. The loss coefficient seems quite ok compared to the experimental data. But (there is always some but unfortunately), there is significant difference of the vortex ring separation frequency (the frequency is lower).

I was using quite long time step (2.5e-5 s), therefore I'm trying to simulate one operating point using 1e-5 s length of time step. It seems quite promising on the other hand the continuity residuals are still quite large (something about 3e-3 at the end of the time step with 40 iterations).

So is there some certain value of the continuity residual when you can assume that the result will be correct?

The second question is about the computational domain, mine one has the outlet part long as ten diameters of the pipe behind the diffuser. Is it enough? And how much can the length of the outlet part of the domain influence the dynamics of the vortex ring separation.

Thank you for any advice and have a nice day

[lihongyang0]

I'm dealing with simulation the cavitation in a Lavel nozzle. I choose the transient, mixture, energy equation and k-e model. Every property of materials is varied with temperature. Each of relaxation factors is about 0.1. The boundary condition is mass flow inlet (13kg/s), pressure outlet (101kPa). The fluent has been calculating for a very long time (110000 steps). But the mass flow on the outlet is about 30~70kg/s. The continuity residual is very high. I have changed many groups of relaxation factors. Now I don't know what can I do to achieve the convergence.

[Kozan]

Hi,
You can find my conference contribution using the following link, may be it will be usefull:
https://www.researchgate.net/publica...VERGING_NOZZLE