Problem for the dc-dc converter dc simulation!

When I a dc analysis for a boost dc-dc converter in Hspice
change the power supply from 2.7v to 4.0v

.dc vdda 2.7 4.0 0.01 /do the dc analysis

I did not use the .ic to set the initaial conditions
but it was aborted.Because it could not converge in the 2.7v
" **error** no convergence in dc sweep curves at 2.7000 "

but when I use .load loading operating point , it still could converge.
.load "E:\xxx.ic0" /loading the operating points

It seems that the ".load " do affect the simulation

Is the using of ".load" right?

And what I want to ask is how to set the initial condition for the dc-dc converter when do the dc analysis in the Hspice?
Are there any other methods to solve the convergence problems?

If someone have successfuly done the dc analysis for dc-dc converter, please help me!
Thanks!

hello, I have simulated boost converter in PSpice but not Hspice. and i have no knowledge in HSpice at all. but in Pspice, if i have a problem with convergence, i would reduce the timestep. hope it helps.

Do you have the simulation error for transient simulation?

If you can simulate the transient analysis, you may get the operating point which may help to solve the dc convergence problem.

What do you mean by DC anaylsis? Switching converter cannot operate without switching, you can only do transient (time domain) analysis on it. If you want to solve the operating point problem in transient analysis, you can use .load for operating point assignment. or you may try to assign reasonable initial condition to the important signal node in your circuit eg. input voltage, output voltage, error amplifier output voltage, ramp signal voltage. Also you should assign initial state to your logic blocks like SR latches/flipflop.

hylas is correct -- dc analysis for a switching power converter does not make sense.
It only makes sense if you are using average models for the power converter. But in this case the switching transistor/diode combination would have to be replaced by an apppropriate model.

Is it possible for you to post the netlist and the output file *.out?

This might give us a better view of what your simulation model actually
looks like.

Best regards,
v_c

Thanks for everybody
firstly I have done the transient simulation successfully and attained the operating point in the xxx.ic0 files. But when I reload it in the dc simulation, it seems no affection the simulation and reported the errors about the convergence.
In order to attain the output voltage vs the input voltage(also the temperature),I do the dc simulation.
If it is no sense to do the dc simulation, how can I attain the output voltage vs input voltage(or the temperature)

Perhaps you can change the input voltage slowly when you do transient simulation. You can get the output voltage which is corresponding to the DC simulation.
And do the same thing at different temperature.

Thanks jwfan
I will do the thing as you told.