[cnqin]

What is the basis for setting "Maximum length scale for area density" in the free surface model? The default value is 1m, but in microscale simulations, the smaller the value, the more stable the solution.

[ghorrocks]

This factor is described in the documentation, so please refer to it.

It is a factor in the inhomogenous multiphase model. It would be unusual to be using this model, normally microscale models use a homogenous multiphase model (with free surface model) and they do not require this factor. Microscale flows do not tend to get the foamy/bubbly regions which you get in metre scale models.

So check that the inhomogenous model is the correct model for your physics.

[cnqin]

Thank you. Both heterogeneous and inheterogeneous models can choose whether or not to set this parameter. As you suggested, I don't need to set this parameter in my microscale simulation.
In addition, I want to know how to improve the interface sharpness, the interface acquired by the free surface model is not clear, even though I set the compression level 2.

[ghorrocks]

Can you describe what you are modelling? Please describe the geometry, what the fluid/fluids are, what flow is imposed and how you have modelled it.

[cnqin]

I simulated the interfacial rise process in a square capillary tube (1um) driven only by interfacial tension force. The fluids are water and oil.

[cnqin]

The viscosity of water and oil phases is consistent, but I found that the interface in the gas-water process is clear. Is this related to the viscosity ratio?

[ghorrocks]

For a 1um duct with oil and water then you definitely do not want the inhomogenous model, you definitely want the homogenous model.

I have done an almost identical capillary rise simulation validation a few years back. Some comments from me:
* The default CFX free surface settings are not optimum for micron scale flows. I recommend you do a little validation exercise on all the free surface settings as you will probably want to change a few of them.
* A key one with the coupled volume fraction solver. I have found that this is much faster, but might cause problems. Test it and see if it helps you.
* Your mesh should have hex elements with an aspect ratio of essentially 1. Even tiny variations in cell aspect ratio means the laplacian pressure will be off by quite a bit.
* You might need a bit finer mesh.
* This needs a double precision solver.
* This is most important one - you will need an amazingly small time step. Adaptive time stepping, homing in on 3-5 coeff loops per iteration is a good start. Larger time steps cause the free surface to smear.

If you are careful you will probably notice some inconsistencies between results. There is a well known singularity with free surface modelling: https://www.sciencedirect.com/scienc...67278906000844

[cnqin]

Thanks for your advice, I will continue to test the simulation.