I set the water injected from a small hole as dispersed fluid and the stationary water in the tank as continuous fluid. The tank is open to atom. and set as opening outlet. The jet length from transient simulations is about half the test data. Any suggestion is highly appreciated!

Hi,

Why are you using a multi-phase simulation when you have only one phase? If you want to track where the inlet water goes use a user scalar. Have a look in the documentation for additional variables.

Glenn Horrocks

Hi Glenn,

Actually this is a simplified case study and eventually the injected liquid has properties slightly different from the liquid in the tank. I noticed the mean diameter of the injected liquid, i.e., water, has a significant impact on the jet growth but I am not sure what a reasonable mean diameter of water jet should be. I can try variour diameters and compare the predictions with some test data but how can this value be general?

Thanks!

Fred

I have the same exact problem. I am injecting a liquid in a tank. I used 1.0E-4m for the mean diameter of the injected liquid. When I used 1.0E-6m, I got different results. I just wonder if someone from CFX can respond to our questions. What is the proper value for mean diameter of water droplet.

Hi,

What multiphase model are you using? Homogenous or inhomogenous? (I think you should be homogeneous) Have you set both fluids as continuous variables? Is the free surface at the top important or can it be ignored?

I could be wrong, but I suspect the diameter parameter is for inhomogeneous simulations for the disperse phase. Your simulation should be homogeneous and both phases should be continuous as you have no discrete phase.

Glenn Horrocks

Thank you for your response. This problem is similar to injecting a colour in a cup of water and you need to trace the plume of the colour with time. If I use homogenous model then I will not be able to see where the injected liquid goes. Correct me if I am wrong. Also how can I get the volume fraction (concentration) of each liquid at certain time by using homogenous model?

Thank you.

Gary

Hi,

You will be able to see where the fluid plume goes with a homogeneous model! The homogeneous model means both phases share the same velocity field, but the volume fraction will vary across the field. You can trace the plume by watching the volume fraction.

Inhomogeneous multiphase is for when there is a different velocity field for different phases, such as droplets in air. The droplets and air interact through momentum transfer, but the droplets have a different velocity field to the air as they are moving relative to the air.

If the injected fluid has the same properties as the main fluid then forget multi-phase entirely and use an additional variable. That will do the inject colour into a cup of water and trace the plume over time thing quickly and easily without all the additional headaches of multi-phase simulation.

Glenn Horrocks

Thank you Glenn. It seems you have experience with this type of problems. Although I am happy with the Inhomogenous model but I like to explore the single phase method. You said I can use single phase flow and additional variable to perform the same simulation. Can you provide more details about how to use the Additional Variable and where (momentum equation ?). Thank you

Gary

Hi,

The documentation discusses additional variables. In CFX10, have a look at tutorial 4, flow from a circular vent.

Glenn Horrocks

Thanks Glenn. Gary