Hi all,

I am trying to simulate a water jet into a supersonic flow (M ~ 3) and not having tons of luck. I am trying simulate an experiment by Baranovsky & Schetz (AIAA-50798-133) which measures the penetration of the liquid into the supersonic flow. If this experiment is reproducible, I would ultimately like use this method on a more complex geometry.

I have the steady state Mach 3 case converged for a square 23 cm wind tunnel that is ~ 1 m long (I have the inlet upstream a bit but am not too concerned with proper tunnel bl growth). Whenever I add the liquid jet, the simulation crashes after 2-4 outer time steps (not inner steps). I have tried many configurations, but I believe the following is really what I would like to use:

Air Ideal Gas - Continuous Fluid Liquid Water - Dispersed Fluid (Droplet size ~ 0.001 m - Not too sure about this)

Buoyancy, Particle Model for Interphase Transfer, and Surface Tension added to allow use of the Grace Drag Model.

Heat Transfer - Total Energy

Standard Free Surface Model. (Not sure about this one either.)

Homogeneous Scalable K-eps turbulence model.

I have tried many permutations of the models above with various timesteps (from 1e-4 to 1e-7) without any progress.

Next, I was going to remake a coarser and a finer mesh and test those out as well, but I wanted a sanity check to see if what I'm trying makes sense. Or perhaps try a slip wall simulation for the tunnel walls in case the boundary layer recirculation is the culprit? Any help or comments are appreciated.

Thanks

-Alex

Follow up: Is this a situation for the MUSIG model? I don't have any experience with this option, but since I am unsure of the droplet size I was thinking this might be a solution.

-Alex

Hi,

Do you have inter phase mass transfer and heat transfer on? I would turn those off and start with inert particles. If that still causes problems then start by doing one-way coupling between the flow and the particles and only introduce full coupling when it is working fine.

When they behave themselves then turn the additional physics on one at a time until the full thing is working.

Glenn Horrocks

Now this is really a very, very complicated simulation. You will need a lot of luck.

- First, swith off buoyancy. Don't think this is really relevant.

- Forget free surface flow. You will get droplets.

- Forget MUSIG initially. Be happy if you get a solution with one droplet size.

- Use minimum volume factions of 1e-5.

- I would not start with a converged Mach 3 solution. I would start with a low gas velocity and try to get a solution with water injection. And then increase throughput.

- If you have a small amount of liquid you could use coupled particle flow.

- If you have a lot of liquid, I would suggest use two continuous phases, mixture length scale 1e-3 to 1e-4 [m]. Does your gas flow suggests Mach 3? What would you expect for a multiphase flow? Do you know the speed of sound for a multi phase mixture?

Gert-Jan

www.bunova.nl

Thanks Gert-Jan and Glenn, I appreciate the advice.

I see two paths forward per your suggestions, and I think both are very good options. I was considering starting at a lower velocity and working towards the final desired velocity, so I will give that a shot. Also, getting one model working at a time should help me limit the possibilities and make some good progress, instead of having so many things to change at once and not really being able to tell if I am moving forward. That is probably good advice in general for utilizing the many models in CFX.

I agree with the luck sentiment, though. This is a code validation experiment to see if CFX can do this and be a useful tool for simulating this environment. If it cannot, then we can continue with our other methods of designing these systems. I was just hoping to add another layer of fidelity to our engineering.

Thanks,

-Alex