[HZ Ting]

I am currently trying to model a multiphase, free surface, high viscosity molten glass flow (5E4Pa.s) through a cylindrical nozzle into a domain of air. The domain, meshing and boundary conditions look very similar to the inkjet tutorial in FLUENT (except that I am I doing it as a 3D, 45 deg axisymmetric segment in CFX).
Using "thermal energy" modelling, the nozzle also has a fixed temperature of 700K while the opening boundary condition has a fixed temperature of 300K.
I am interested in understanding how the heat transfer affect the resultant flow profile.
The solution converges when air is specified at "air at 25C" which I assume is invalid for my case. However, when I tried using "air Ideal Gas", I am unable to reach convergence. The error shown is "fatal linear solver error." I have read the FAQ section of the wiki, yet I am quite confident with my hexahedral structured mesh and my boundary conditions. I have checked the locations where the local volume fraction RMS are high (right at the junction of the nozzle) but refining the mesh there doesn't seem to help. Are there any suggestions?

[ghorrocks]

5e-4 Pa.s is not high viscosity. That viscosity is less than water. Are you sure you have the viscosity correct? I would expect molten glass to have a much higher viscosity than that.

Modelling MEMS structures is a very different world to modelling normal engineering structures in the mm and metres scale. You need to consider different things and the normal rules of thumb do not work.

But first of all, why are you modelling air as an ideal gas? You might need to attach a drawing to show it. I have done many MEMS models over the years and it is very rare that I need to consider the compressibility of air. So please explain why you need to model an ideal gas in your case.

And a key thing about MEMS modelling in CFX is that the linearisation of the surface tension term is not very good. This means that flows strongly dominated by surface tension (which is most MEMS flows) converge poorly on CFX. The only way to fix this is to use very small time steps (time steps of 1e-8 to 1e-10 s). This is the reason Fluent has a clear advantage over CFX in MEMS modelling, its surface tension model is much better than CFX and runs much faster.

[HZ Ting]

Thanks for your reply. I have attached a picture of my setup. I am working with a viscosity of 50,000 Pa·s and have neglected surface tension (ST), assuming it to be negligible under such high viscosities. (I tried including ST and as you pointed out, it wasn't successful).

I have attempted to model the same configuration in 2D using FLUENT, but I am encountering worse convergence compared to CFX at this viscosity.

My understanding is that there will be significant heat transfer from the high-temperature setup. I am using ideal gas to capture the air density change, which in turn affects the air flow velocity, the heat transfer and the temperature dependent glass viscosity.

[ghorrocks]

Oh, the viscosity is 5E+4, not 5E-4. I did not have my glasses on when I read that . In that case, yes, it is high viscosity.

The nozzle is only 1mm radius, that is not very small for a MEMS device. The nozzle on my MEMS device is 12um diameter - that is a lot smaller. But still, with your high viscosity and low flow speed the Reynolds number of this flow is going to be very low. CFX can have problems with very low Re numbers, but I think this should be OK.

Yes, at 700K you will get significant ideal gas effects, so I think you are correct to model this with an ideal gas.

Can you attach an output file of a failed run?

Also - try lowering the time step size. Compressible gasses introduce an acoustic time step limitation, so if you are just using the same time step as the incompressible simulation it is not a surprise it failed. You could play it safe and just use an adaptive time step size set by Courant number, and use Courant number of 1.0. That will give you really small time steps.