CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   Changing Boundary: Decreasing Inlet Velocity - Convergence Issues (http://www.cfd-online.com/Forums/fluent/84870-changing-boundary-decreasing-inlet-velocity-convergence-issues.html)

VT_Bromley February 10, 2011 11:09

Changing Boundary: Decreasing Inlet Velocity - Convergence Issues
 
Hey all,

My system is a multiphase flow problem with sand and air. The air is injected through a nozzle initially with a set velocity of 345 m/s. After 0.1 seconds I would like to stop the inlet velocity or decrease it to approximately 0 m/s and let the sand settle. I ran the simulation to 0.1 seconds then manually changed the inlet velocity and began the calculation again.

Currently I have tried adaptive meshing, variable time stepping, and slowly manually stepping down the inlet velocity with no luck. I cannot get the problem to consistently converge. Does anyone have any recommendations?

Thanks,
Mike

alastormoody11 February 11, 2011 01:32

Hi,

try reducing the under-relaxation factors of the problematic equations.

Also since you are modeling sand in air I am assuming that the you are using the Lagrangian- Eulerian model which requires high grid resolution depending on the particle size so maybe instead of adaptive meshing look at the unconvergerd solution for places where the concentration of sand is high and try with a finer mesh in those places from the start.

The grid required for an accurate solution would have a pretty high cell count if the sand is dispersing in a large portion of your control volume.

Amir February 11, 2011 03:08

Hi Mike,
for solving such Lagrangian-Eulerian problems you can implement EDEM plugin in FLUENT.
I've never used that before but you can see it's propaganda.
http://www.dem-solutions.com/

ComputerGuy February 12, 2011 09:02

Mike,
What size sand are you simulating? What time steps are you trying to use?

Unlike alastormoody, I think you can simulate this with a two-phase (or N-phase) Eulerian-Eulerian model. I don't believe there's a need to resolve individual grains of sand. At any rate, here are my suggestions:

1) Ensure that your grid is adequate in places it needs it
2) Ensure that when you begin your velocity ramp (or step change) that you were working with a converged solution in the first place. Obtaining convergence with a step-changed boundary condition off of a non-converged solution is just asking for trouble.
3) Is the physics really a step change? Meaning, does the velocity go from something to nothing instantaneously? In my experience, having a ramp, albeit a fast one, can improve the convergence of the solution. It takes longer to solve, but an unconverged solution is worthless.
4) If you need a UDF that will ramp down the velocity, let me know.
5) Take small time steps during the ramp, and much smaller time steps after you have zero velocity. Remember, fluent is trying to solve flow. It isn't a "no flow" solver. You'll struggle to get a converged solution if you don't take tiny time steps until all of your sand settles
6) If your sand size is too small (sub-micron), it's going to be tough to converge and see everything settle, as minor turbulence will keep grains aloft.

Have a look at the residuals and let us know what's misbehaving. In my experience, when simulating granular flow, epsilon (from a k-e turbulence model) tends to wander.

Regards,
ComputerGuy


All times are GMT -4. The time now is 14:29.