There are 4 approaches to running an implicit analysis first, followed by an explicit analysis.
After running the implicit analysis, submit the explicit analysis as a full deck restart. (See attached input files.) This is a very general approach in that it allows various changes to be made to the model, e.g., adding or deleting parts, or adding/changing boundary conditions or loads.
Include the keyword *INTERFACE_SPRINGBACK_DYNA3D in the implicit analysis input deck. This will create an output file named ‘dynain‘ at the end of the simulation, which contains deformed geometry and initial stress data in keyword format. Merge this file into the original input deck (replace the original *NODE and *ELEMENT_SHELL commands), de-select the implicit options, and run the stress-initialized, explicit simulation. No restarting is required; the explicit run constitutes a brand new analysis which has been intialized according to the results of the precurser implicit analysis. Note that the dynain file does not initialize beams or discrete elements and also does not initialize contact forces.
You can specify a load curve which indicates which time intervals are run implicitly, and which are run explicitly. The abscissa of the curve is time and the ordinate is 1.0 during periods the solution is to be implicit and 0.0 during periods when the solution is to be explicit (curve is a step function). Set IMFLAG in *CONTROL_IMPLICIT_GENERAL to -|curve ID|. Switching from one analysis to the other is seamless and has no CPU or I/O overhead.