Convergence issues using the multiphase VOF model and the pressure-based pseudo transient solver

  • 44 Views
  • Last Post 05 December 2019
  • Topic Is Solved
rachels1001 posted this 02 December 2019

Hey guys,

I am trying to model a perforation in the side of a pipeline. The pipeline has gas flowing through the main body, with water in the perforation. I am interested in the interface between the water and gas, and so I am using the VOF multiphase model, as the flow is stratified. Because I am implementing the VOF model, I am using the pressure-based pseudo transient solver. I am also using the standard k-omega turbulence model because I am interested in eddy formation. 

I am experiencing convergence issues with this simulation. Namely, whenever I run it using either the iterate or dual-time-iterate command, I get the following errors:

"Experiencing convergence difficulties-temporarily relaxing adn trying again...

Divergence detected in AMG solver: pressure coupled / k / omega / phase-1-species-0...etc.

These errors are given immediately, prior to any iterations completing. 

I have adjusted my URFs and flow courant number. I am using the following values, and still experiencing these errors:

Flow courant number: 10

Momentum/pressure: 0.5

Density: 0.25

Body forces: 0.75

Turbulence kinetic energy: 0.5

Turbulent viscosity: 0.75

Energy: 0.5

Phase species: 0.75.

I am using the variable time stepping method.

Is there any other things I should try to do to improve convergence? Or, as I am getting these errors, is it probably something wrong with my mesh or setup? Another thing that I am worried about is that my model does have cell zones that contain solid sections, could that be incompatible with the VOF model?

Thanks so much for the help!

Claire

Order By: Standard | Newest | Votes
rwoolhou posted this 03 December 2019

How much mesh have you got in the perforation? If you look at the velocity there & cell size how long does it take for the flow to cross one cell? Remember you'll need 5-10 cells across the liquid jet and any droplets to capture the free surface. 

rachels1001 posted this 04 December 2019

I had around 20 cells across the 3mm diameter of the perforation. The length of the perforation is 12mm, and there is 100 layers of cells along the length of the perforation. There is also 20 inflation layers in the gas pipeline before the perforation. 

Removing the solid cell zones did help; however, the simulation still diverges after a short period.

rwoolhou posted this 05 December 2019

If you look at the results just before it goes wrong can you see anything "odd"?  Also, does the free surface pass through (as opposed to along) the inflation region?

rachels1001 posted this 05 December 2019

Hey guys, thanks for the help!

 

I tried a couple things today, but what eventually worked was refining my mesh even more and converting the mesh to polyhedral elements once I was in fluent. From there, decreasing the under-relaxation factors and courant number and slowly increasing them over the run worked out pretty well.

 

 

Close