I am modelling the shape of a droplet when it hit the substrate in thermal spray coating. I am thinking of using particle tracking to model it. Anybody know how to set up a model. Pls. help me. I am quite new to CFX..

In the beginning, I created a plate and enclosue it by air. Then I crate a domain for plate (solid) and air (liquid) with heat transfer setting as well. Is it correct for particle tracking? I have velocity of the droplet, droplet diameter, initial temperature.

Anybody know something, pls. help me.

Thank you very much for your help

Hallo,

Well, I am not a specialist on this kind of simulation, but lets try to help. First thing, I don´t think that particle tracking is suitable for this case (since you want to see only one droplet). If you want to see what happens with one droplet when it touches the substrate, then you will need a eulerian-eurelian approach.

It is not a simply case, but I would try: - only one domain (you are not interested in the plate), like a cube with the size scale similar to your droplet size, with one of the faces as BC Wall (the substrate) and the 5 others as BC Openning. - the domain with two substances: air and the one of your droplet. - a good inital values definition. This is the point where you define the initial shape of your droplet. Try to calculate the Weber number of it...if this is small ( 1 ), considering it spherical is not bad. Then you must create a function to set the values of concentration of your droplet in the domain (1 inside the droplet and 0 outside). Check the tutorial with the free surface flow aver the bump for more details. - then a transient simulation with really small timesteps.

I think you will need really accurate values for the variables (as surface tension and viscosity) as a function of temperture to get a reliable result.

Hope it helps

Anderson T F

There is a tutorial named "Butterfly valve" that covers the particle tracking set-up. -Dr. Flow Squad http://tinyurl.com/2gkjh8

Thank for your reply, Anderson. However, in the case I would like to model the heat transfer and droplet deformation in one model, can I use the method as your advise.

If I model droplet on the substrate as yours, how can I set up "create a function to set the values of concentration of your droplet in the domain" what does it mean?

All the data I had includes initial temperature of droplet (at very high temperature), substrate, surface tension of droplet, initial shape of droplet is sphere. When the droplet hit the substrate, there will be heat transfer between them and then the droplet will deform from a sphere to a layer on the substrate.

I am very appreciate your help.

Hallo,

Sorry about not replying first, but I was enjoying some holidays in Greece.

First thing, I would start my simulation easier (old motto: "start simple, improve later"), focusing on only one detail. In this case, I would put off my worries about the substrate and simulate first only one droplet hitting it (even because it will be a lot of process effort to simulate many droplets).

So, to your questions:

1 - Using the heat transfer coefficient would be nice, but I don´t think you will find this value easily. Anyway, try to guess it from some source (even as a constant value, just to start) and later you check if your results are very sensitive to this parameter (let´s hope not ).

2 - The opening BC are there just because you need to set something. So, try to make them affect as little as possible your simulation. Set all the parameters to be as similar as possible to the domain.

3 â€" How to crate a droplet in your domain: For further details on this question, check the tutorial about free surface over a bump. In short words: you will create a function which models a sphere inside your domain. Then you create a step function with the previous one and the values: 1 for inside the sphere and 0 for outside. Finally, in initialization, you set the values of concentration of your liquid to be the result of this step function. This way you will create a sphere which is inside your droplet (100% liquid) and outside air (100%).

About Nusselt: hard one. Has to do with your heat coefficients and will change with temperature. Try to use the default values in the beginning and later you solve this problem.

About Drag forces: no worries for now. If you simulate only one droplet falling on your surface, drag is not important(in your initialization, make the droplet start already almost touching the surface). Use the simplest approach, Schiller Naumman I think.

About initial values of T and velocity. I dont know your case, but if the droplets are small and they have some time to interact with the turbulent air, probably they will all be at the same T (anyway, start with isothermal conditions sounds better for me, it is easier). Velocity: air =0 and droplet=something small in the direction of the surface, just to make sure they will touch.

To sum up: start easy! Your case is not a beginner's one. You will come across a number of parameters whose value you don´t know. Just set them for the simplest condition possible (normally the default) and try to get some result. Afterwards, make sure you will come back to every single one of these parameters and test the sensibility of your result to them (probably your result wont be sensitive to many of them). When you find a parameter that is important for you result, then you care about it (lab experiments, literature, other simulations, etc etc ).

Keep me updated of your progress

Have fun

Anderson T F