I have a transient multiphase simulation with mesh deformation. (See attached pictures) Problem is that the turbulence equations keep diverging. I am modelling a set of water locks that slowly fill with a set of barges inside. The mesh deformation models the movement of the barges with the rising water level. Mesh deformation is linked to move with the position of the average water level. (I defined it on a velocity basis to ensure I got the initial mesh velocity with my first iterations.) No matter what I do, the problem is the same thing every time. I get a good initialization, and then as I step through time, the turbulence residuals slowly get larger. Eventually, after 20 - 120 time steps, depending on what settings I use, the model blows up and crashes. Any ideas why this is happening, and what I can do to stop it?
I have tried k-e, k-w, and Spalart-Allmaras. Currently I am using Spalart-Allmaras to try and get it stable. I have an under-relaxation factor 0.60 for my turbulence solver. I have added a linear ramp to the solver, with an initial value of 0.20 ramping up to 0.60 over 12 iterations. No matter what I do, the simulation eventually diverges, and only with turbulence. All other residuals show strong convergence. Further, I only have problems with my lower region (the bottom region shown in my pictures.) This is where the water enters through an extensive set of pipes. The pipes are meant to stop the water velocity and create smooth flow into the lock.
Some simulation settings:
Rough reynolds number: 1.55x10^5
Average cell size: 5.0 ft
Average surface cell size: 1.0 ft
Timestep: 0.05 s
Iterations between timestep: 45 (120 on initialization)
Total solution time: 32.0 s
I usually fix my diverging turbulence by reducing the relaxation factor for the turbulent viscosity to 0.1 and increasing the max viscosity ratio a couple of orders of magnitude.
couple of suggestions in random order of importance
make sure you mesh is good, avoid highly skewed elements and big differences in volume of contiguous cells
make sure your courant number is sensible
try to link the timestepping advancement not on the number of iterations, but on the residual. some timestep might require more iterations to get convergence.
if the movement of the barges is fast, compared to the mesh size, try reducing the timestep.
Thanks for the advice all. In the end, I reduced my timestep by an order of magnitude and that fixed all my problems. I probably didn't need to cut it by a full factor of 10, but I'm working with limited computer resources. It takes me sooooo long to test any change that I'm happy to just leave it where I know it will definitely be stable.
|All times are GMT -4. The time now is 02:17.|