Reno Genest
Ansys Employee


Are you running an explicit dynamics analysis? Or an implicit static (or dynamic) analysis?

If  you want to run an implicit static analysis with a constant timestep, make sure the following are set:

  1. Set IMFLAG=1 and DT0=initial timestep on *CONTROL_IMPLICIT_GENERAL. The default for IMFLAG=0 which will result in an explicit  analysis.
  2. Set IAUTO=0 for a constant timestep on *CONTROL_IMPLICIT_AUTO. 

Refer to the LS-DYNA user manual Vol. I for more information in implicit keywords:

The above should set  a constant timestep. 

Also, why is your implicit initial timestep set to 2.75e-5 second? This is a very small timestep for an implicit solution. This timestep is more typical in explicit dynamics simulations. What is the termination time for this implicit analysis? For example, a termination time of 1 second is very common for implicit static problems. Note that in implicit static, time is not real and not taken into account. With a termination time of 1 second, an implicit timestep of 0.1s or 0.01  is typical. You can use a timestep of 0.001 if you run into convergence issues. With a very small timestep (2.75e-5 second), it will take a long time for the solver to converge to a solution, especially if your termination time is 1 seconds or more.

Note that if you run explicit dynamics, the timestep is set by the solver based on the smallest element in your model (element characteristic length), the material stiffness and density (E and rho), and the TSSFAC parameter (default=0.9) on *CONTROL_TIMESTEP. The explicit time step  is governed by the CFL stability criteria:


Let me know how it goes.