To address the divergence, I’ve already attempted several of the troubleshooting methods suggested in the manual (https://mfix.netl.doe.gov/doc/mfix/23.4/html/faq.html#what-do-i-do-if-a-run-does-not-converge), but to no avail. Upon reviewing my results, I noticed that the gas phase volume fraction was lower than the packd bed void fraction. Additionally, as mentioned in the manual, the pressure residuals were not decreasing satisfactorily.
I’ve tried increasing the number of iterations for the pressure term and reducing the under-relaxation factor for the volume fraction, among other suggestions from the manual. Despite these efforts, the problem persists.
Given that those parameters, such as the angle of internal friction and the restitution coefficient, were directly provided rather than derived from experimental data, I am beginning to suspect that the values used for these parameters may be inappropriate or unrealistic.
Could anyone here assist me in reviewing my case setup? Any advice on how to better tune these parameters or any other suggestions would be greatly appreciated.
Thank you very much for your time and consideration.
Thanks. It’s very helpful to provide this sort of information when reporting a problem, in addition to just the project file. This is why we have “Submit bug report” in the main menu, this creates a ZIP file containing all logs and relevent info, in addition to the mfx file itself. Thank you.
>>>>>#################################################################
ERROR from iterate.f:1027
DT_FAC >= 1. Recovery not possible!
<<<<<#################################################################
You should not use a time step factor of 1. Please try with the default value of 0.9. When DT_FACT=1 MFiX will quit if there is a lack of convergence or unphysical result. Leaving the default value DT_FAC=1 will let the time step go down when convergence is difficult and increase the time step when convergence is achieved quickly.
The original test.mfx attached to the first post in this thread has a DT_FAC of 0.9. I ran this for 16 hours and reproduced the reported error.
Here are plots of simulation time, DT, and residuals
The residuals follow a very regular pattern until the failure at the end of the run, where DT goes below DT_MIN.
I’m not sure exactly what’s happening here but it’s noteworthy that right before the failure, there were 55 warnings about excessive fluid velocity. I suspect this is the reason for the divergence:
You could try adjusting MAX_INLET_VEL_FAC as the warning suggests. Or perhaps something is wrong with the model setup, leading to excessive velocity in this cell.
@wuming: I increased MAX_INLET_VEL_FAC to 10 as suggested in the warning, and I get past the problem at 0.9s.
You can use the “locate keyword” feature (spyglass icon) if you don’t know where the control is for a keyword. Or highlight any keyword in a message and right-click to bring up the context menu and select “Help”
