Help about Hspice ".save & .load" command

[peter_hawk]

hspice save load

I use .save and .load to speed up the simulation .

in first step , I save the operating point for initial condition
.tran 1u 62.09m
.save type=.nodeset file=top.ic time=62.09m

in secend step, I use .load command
.tran .1n 62.1m
.load file=top.ic

but Hspice seems to simulate the circuit from time=0

Can any one give me some advise?
Thanks a lot

 

[xwcwc1234]

hspice .save

May be you need additional command in Hspice, the command .nodeset

 

[ahmadyan]

Re: hspice save load

I know it is probably too late, but for the records:

To resume the simulation in hspice, you've to force the initial condition. Using default tran and nodeset will allow the hspice to use your initial conditions as "guess" for the newton method in DC analysis (even when you don't use the .op) to compute the DC operating point (which normally end up in the standard dc operating point, hence simulation would resume from time 0 )

To bypass this and force the simulation to start from later time (like 62.09m in this example), first use the .IC command, not the .nodeset (in .save, you can specify the .ic type instead of .nodeset),
also use the uic mode for transient simulation, hence

.ic v(1)=1 v(2)=2 i(L)=3 ...
.tran t0 t1 uic

This will do the trick.

I use .save and .load to speed up the simulation .

in first step , I save the operating point for initial condition
.tran 1u 62.09m
.save type=.nodeset file=top.ic time=62.09m

in secend step, I use .load command
.tran .1n 62.1m
.load file=top.ic

but Hspice seems to simulate the circuit from time=0

Can any one give me some advise?
Thanks a lot