Another problem on Lt spice. I would like to know if I use the options uic in transient analysis but I don't specify the .IC (the initials conditions), what IC will use Lt spice for the resolution?

I did that and it ran but I was not able to see a file with DC point information.

Another question? why will a simulation fail to find the dc operating point?

  • \$\begingroup\$ Do you have a circuit that caused DC analysis to fail? Can you share it? \$\endgroup\$
    – The Photon
    Feb 15, 2018 at 17:29

1 Answer 1


The use of UIC means that Spice will not go through the "initial transient solution" step (so-called "ITS") to find the DC solution at \$t=0\$.

When you use UIC, the initial value of every single energy storage (voltage and current) device is treated as zero, except for those which are explicitly provided using the .IC statement.

If you know, a priori, all of the initial values for the energy storage devices in the circuit, you can use UIC to compute the steady state solution without the transient response leading up to it (that may occur if you instead allowed Spice to first perform the ITS step by not using UIC.)

I'm a little confused about your question about not finding DC information. There is a DC operating point mode in Spice that provides such information. It's just not the .TRAN mode. It's .OP, instead.

However, if you are having trouble finding the DC operating point with Spice (such as with some bistable circuits), it may be because Spice assumes that all node voltages start out at \$0\:\text{V}\$ (relative to your ground reference, of course, where ever you placed it.) In these cases, you can use .NODESET to establish node voltages to help Spice find a specific DC solution. (Just don't use .NODESET to set the exact value you get from a previous run! Instead, just set the node voltage "near" to where you think it will arrive, later, and let Spice find the DC solution for you.)

  • \$\begingroup\$ thank you @jonk for the answer. I think that I had a problem with my computer. I will run a same simulation and sometimes it will find the results, and if I run it again, the log will tell me that time step too small or that it can't find the .op point. I simulate on another computer and it seems to work. \$\endgroup\$
    – A. S-S
    Feb 16, 2018 at 15:38
  • \$\begingroup\$ @A.S-S Different simulators have different numerical solution "tweeks" that are not the same as each other. LTspice includes a way to select between a few different methods, too. So there is always that possibility to try. Sometimes, one method will work where another doesn't. \$\endgroup\$
    – jonk
    Feb 16, 2018 at 18:39

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.