Use transient sim operating point for a AC sim in hspice

[seamoss]

I wanted to see how I can use operating point info obtained from a transient simulation (at a given time) for a AC simulation in HSPICE?

 

[erikl]

This is possible with the SPECTRE simulator, but I don't know if it will work with HSPICE: View attachment AC-simulation_on_prevoppoint.pdf

 

[erikl]

Seems it should work with the .SAVE and .LOAD mechanism:

.SAVE [FILE=design.ic0] 
.LOAD [FILE=design.ic0] [RUN=PREVIOUS]

either give the filename or RUN=PREVIOUS

s. hspice command reference

 

[dick_freebird]

I have seen other SPICE simulators (not exactly mainstream, but
2G6 based originally) which had transient endpoint node voltage
store function, and this could be forced as an initial condition
the same as a stored DC solution.

However, you should beware the likelihood that your transient
endpoint is not truly small-signal-settled at every node, and
thus the result may not be the same as what a DC analysis
would give. On the other hand there are many circuits which
a DC solution can't put into the right state (not without a lot
of detail node-setting). For these it might be good to get the
transient final condition, and then "scrub" that through a DC
solution (use it as an initial, then store the DC, then use that
as the initial for the AC analysis). You would refine the DC
that way, but get the benefits of having the transient take
you where you wanted to be state-wise.