Frequently Asked Questions

Can I run <em>Cobalt</em> in local time-stepping mode?
No. Cobalt always runs with global time-stepping.  By specifying a time-step, Cobalt will use that time to advance the simulation each iteration.  By specifying a CFL, the global minimum time step is calculated such that the specified CFL is never exceeded in any cell.  This global minimum time step is then used in every cell.

We have found that the disadvantages of local time-stepping outweigh its advantages.  Local time-stepping’s sole advantage is a reduction in solution time to steady-state cases. However, we never witnessed more than a 20% reduction in run time.  On the flip side, however, local time-stepping can give very poor results for cases that are somewhat close to being unsteady — a truly steady solution may be predicted as unsteady, and a truly unsteady solution may be predicted as a steady solution.  To save both users and ourselves from these uncertainties, Cobalt does not use local time-stepping.

I specified motion but I am not seeing any motion of the geometry when viewing the flow visualization files?

Check to make sure your time start specified in the motion file falls within the expected time range of the simulation.  Remember that one can restart with Option #3 that will reset the solution time to 0.  Also check to see whether you specified a ‘1’ in Data in Lab Reference Frame under Flow Visualization Parameters in the job file.

While the job is running, inspect the ‘total_gridxxxx.cnvrg’ file to see if it shows any change in orientation and position.

My solution is converging very slowly, how can I speed it up?
Try to lower the temporal damping coefficients. Lower the coefficients as much as you can without the solution blowing up, or becoming very noisy.  Generally, the advection temporal damping is the primary ‘knob’ here.   The advection temporal damping generally must be increased above the default value of 0.05 for hypersonic cases, with the highest value, known to us, of 0.12 for a hypersonic case with very strong rarefaction waves. Generally, over the Mach range of roughly [0.1,4.0], the advection temporal damping can be significantly reduced from the default value.  Frequently, values less than 0.01 are sufficient.  Finally, for low Mach numbers, below about 0.1 the advection damping often needs to be in the 0.01 to 0.03 range.  The above values for Mach number and advection temporal damping given above are meant to be guidelines only.  Both grid quality and flow details have a significant impact on the value of the advection temporal damping coefficient needed for stability.

For the diffusion temporal damping, a value of 0.0 almost always is sufficient for all cases except hypersonic cases with isothermal solid walls.  In those conditions, a value of 0.01 has worked well for all cases but one (and that one case required 0.02), to our knowledge.

Finally, if you are specifying CFL, the calculated global time-step may be very small due to extremely small grid cells.  An option is to specify a time-step of 0.05 and run for a few hundred iterations to flush out large transients.  Then restart with either specifying CFL or using your ideal time-step based on your solution.

Why is DR/DT not converging to zero?
For a 1st order solution, it will converge to zero.  For a 2nd order solution, DR/DT should drop two or three orders of magnitude.  As mentioned elsewhere in this manual, this is due to the discontinuous nature of a part of the spatial operator used in Cobalt.

You can also monitor y+ (for viscous simulations), the number of supersonic cells, and moments and forces in the out file.

Can I run a simulation with 10 Newton sub-iterations?
Yes, but there is negligible benefit in running with more than 5.  For steady-state simulations, use 1 Newton sub-iteration.  For time-accurate calculations, use 2 or 3 Newton sub-iterations.  We recommend 3 to 5 Newton sub-iterations when using rigid-body motion.

If the solution does not show the desired temporal accuracy when using 5 Newton sub-iterations, then decrease the CFL or time-step.

My job cannot get past the first several iterations – I get a warning that says non-physical cells.
You may want to raise the advection damping coefficient.  Or use a CFL ramp or time-step ramp (depending on whether you are specifying CFL or time-step).  Because of the combination of flow conditions and grid, it is sometimes difficult to start a solution from initial conditions with a large CFL.  Once the solution has passed the transient start-up stage, then a large CFL can be used.  A CFL ramp or time-step ramp is provided to alleviate start-up problems.
I’m having problems with my <em>Cobalt</em> jobs not running to completion. What does Cobalt Solutions need to help me investigate the problem?
Please send the job file, the out file, the boundary condition file, and any standard *.e and *.o files to support@cobaltcfd.com
Where can I find help for RLM license administration?
Please see: RLM support