Reply To: “Time step is too small”

[Chris Quan]

"Time step too small" is shown when the current time step is less than 10% of the initial time step. When you see the error message about “time step too small”, you need to find out which element controls the time step.  This can be found from the file "admodel.log" in the solver data directory. 

 

If it is the Lagrange element that controls the time step, you need to examine the deformation of the parts to see if there are any distorted elements. If the element controlling the time step is from a severely distorted element, you need to activate erosion controls under Analysis Settings to erode the highly distorted element.

 

Since the End Time in your Analysis Settings is quite short, can you plot Energy Summary under Solution Information? Can you plot Total Velocity by right click on Solution -> Total Deformation -> Total Velocity? Is the total kinetic energy large, comparing with the total internal energy? Is the total velocity large, for example, > 10 m/s?

 

If one of the answers is yes, you need to slow down the motion by increasing the End Time and adjusting the boundary conditions accordingly. This is because you are modeling a quasi-static event. You want to minimize the dynamic motions and make sure all external work have contributed to stress/strain (internal energy), rather than velocity/acceleration (kinetic energy).