How to simulate DC sweep after TRAN?

In which tool? In which version? In which simulator? Are you using ADE? Are  you using the simulator on the command line? 

People cannot read your mind...

As a wild guess as to what you're really asking, if it's ADE and IC5141 (and you're using spectre), there's a field on the Setup->Environment form called analysis order - you can type in "tran dc" to set the order. In IC61X, you can simply drag and drop the analyses in the analyses pane in ADE to change the order they run in.

Regards,

Andrew.

I use your first way to set up.But the results of DC sweep simulation  is at the initial operating points of TRAN.  

And I can't  drag and drop the DC analyse below the TRAN analyse in the analyses pane. 

DC SWEEP can't run at the final operating points of TRAN simulation.

Can you give me more suggestions?

Thank you very much! 

You can't drag and drop if you're using IC5141. You can only use the analysisOrder approach. You didn't say which version you were using (see the forum guidelines, please), so I had to give both options.

You also didn't explain that  you were trying to utilize the final operating point of the transient to start the DC.

First of all, does your DC start from precisely the same conditions as are in place at the end of the transient (in other words, the value of all inputs and also the values of the thing you're sweeping must correspond to the  value it was at the end of the transient). If it doesn't match, then using the oppoint doesn't make much sense.

Other things to try:

1. In the additional parameters at the bottom of the DC options form, type "useprevic=ns" (or "useprevic=yes").
2. In the transient, the writefinal is probably set to "spectre.fc" (see the transient options form). On the DC options form, set readns to "spectre.fc" (i.e. the same file name).

Regards,

Andrew.