[ocyee]

Hello guys, I had been trying to use CFX flow to model a single water droplet with a sinusoidal velocity applying on its base. However, I realized that the velocities value is always zero while running the analysis. I think there might be some mistakes or some other reasons while I try to apply the settings. Can anyone briefly summarise the settings and option that I should work with? Thanks in advance!

[ghorrocks]

Please post an image of what you are modelling and your output file.

[ocyee]

Originally Posted by ghorrocks

Please post an image of what you are modelling and your output file.

Hello ghorrocks, thank you for the reply. I had managed to fix some settings and able to see some results at the CFD post. Im not too sure what Im doing is correct or not, but i will briefly talk about what im working on.

I want to simulate a single water droplet with vibrating condition underneath the base of the droplet. I would like to observe the internal flow of the droplet, ignoring how the surface would react with air too (no multiphase). I had attached a simple slide to summarise what settings that I had used in the analysis, I am not too sure whether im applying the correct settings and boundary conditions or not. I had used inlet veloicty with a sinusoidal function to model the vibrating condition, and a shear free wall boundary to model the stress free condiiton on the droplet surface. I had also uploaded my output file as well. Would appreciate some feedback and guidance. Thank you in advance!

The slide can be found from this link below, file size too big to be uploaded:
https://drive.google.com/open?id=17S...ddtJlZ5EjX7-qP

[ghorrocks]

I can tell you what the flow will be: nothing. That is because if you define the outer surface of the drop to not move then moving the drop up and down will not generate any flow. That is because there is no horizontal density gradient to cause flows. The vertical density gradient does not generate a flow providing you are below the threshold to give Rayliegh-Taylor instabilities (https://en.wikipedia.org/wiki/Raylei...or_instability), but I suspect in your case you are miles away from that (but it is a good idea if you checked).

Why didn't the simulation get nothing? Because you used a inlet boundary on the bottom which is not correct, you need to use moving mesh. And add to that some numerical errors and you get the result you got.

In reality, if you oscillate the drop up and down the free surface is going to move which allows the fluid to move up and down and a flow gets generated from that. You are going to have to do a free surface model to capture these effects.

[ocyee]

Originally Posted by ghorrocks

I can tell you what the flow will be: nothing. That is because if you define the outer surface of the drop to not move then moving the drop up and down will not generate any flow. That is because there is no horizontal density gradient to cause flows. The vertical density gradient does not generate a flow providing you are below the threshold to give Rayliegh-Taylor instabilities (https://en.wikipedia.org/wiki/Raylei...or_instability), but I suspect in your case you are miles away from that (but it is a good idea if you checked).

Why didn't the simulation get nothing? Because you used a inlet boundary on the bottom which is not correct, you need to use moving mesh. And add to that some numerical errors and you get the result you got.

In reality, if you oscillate the drop up and down the free surface is going to move which allows the fluid to move up and down and a flow gets generated from that. You are going to have to do a free surface model to capture these effects.

Thank you for the feedback, just to wrap up from what you had suggested. What I had so far from the results does not prove anything that I want to find. So, if i want to model the internal flow of my droplet, these are the couple things that i need to make changes to model:
1. assign a moving mesh to the droplet base.
2. assign a free surface model to the droplet surface.
Am I right?

How about the total energy model and buoyancy model that I applied, will that be appropriate, and also is the steady state analysis enough or should i switch to a transient study? Sorry for any inconvenience caused, I am still a new user to CFX. But appreciate the feedback!

Finally: You will find this simulation much easier and quicker in Fluent. It has much better free surface models for surface tension simulations than CFX (by an order of magnitude).

[ghorrocks]

This flow is inherently transient, you cannot model it steady state.

It is unlikely you need total energy for this. Just use constant properties for water and air (unless you have a good reason not too).

Yes, you need a free surface model with surface tension. Be aware the surface tension model is very tricky to use - I recommend you do some validation tests (eg Laplacian pressure in a stationary drop) before you use it for a real run. You will find it is VERY sensitive to mesh quality and time step size.

Yes, you will need to use moving mesh. You need to model what is actually happening.

A nice advantage of this is that your mesh can be a 2D slice using a quad mesh with 1:1 aspect ratio, swept around a small angle. You will need the 1:1 aspect ratio, as you will find in your Laplacian pressure validation You will not be able to model this accurately with a tet or tri mesh.

You will need tiny wheeny time steps. Don't guess what you need, you will get it wrong. Use adaptive time stepping homing in on 3-5 coeff loops per iteration, so it finds the time step you need automatically.

[ocyee]

The total energy model is what my supervisor suggested me to use, because to actually model a compressible flow and include the kinetic energy effect for water behavior.

Just one last thing that I am not quite understand about is the 2d slice meshing part that you had mentioned, are you talking about the meshing method that I had applied on my water droplet model? Can you elaborate more on that?

[ghorrocks]

? The kinetic energy effect of water is the Bernoulli Equation and that applies to incompressible flows as well.

The speed of sound in water is about 1500m/s. You are only vibrating at 0.1m/s, which is a Mach number of 6e-5. The normal rule of thumb is that the Mach number needs to be greater than 0.3 for compressible effects to be significant. You are far too slow for the Mach number to be high enough for compressible effects to be significant.

Can I humbly suggest your supervisor is wrong?

2D meshing: https://www.cfd-online.com/Wiki/Ansy...tion_in_CFX.3F