[SOLVED] Singular Matrix error on LTSpice

[schmitt trigger]

There is a power supply circuit which we have built over 70,000 units in almost 9 years. And it has been working reliably for all that time, even during extreme environmental conditions.

We would like to reuse this circuit for an almost identical application. We actually have built several dozen prototypes and they work just fine. But we would like to understand the actual operating conditions, and make sure that we are not overloading something.
The best way to do this is through simulation.

Since this is an LT3433 buck-boost regulator, I used LTSpice.

When I run it, however, I get a "Singular Matrix error on Node 006"....Node 006 is only the 330pF compensation cap to ground.

Now, PLEASE NOTE: My question is only related to the LTSpice error message. The real circuit itself is working very well.

EDIT: I had to upload the .ASC file as .TXT file, for the attachment manager to allow me to upload it.

 

[mtwieg]

When I run it I get the old "damped pseudo transient" message, which usually means it's unable to converge to an initial DC condition. I solved it by forcing an initial condition on that node voltage. So label that net "vc" and then add the statement ".ic V(vc)=0" and it works.

 

[BradtheRad]

Besides setting an initial charge on the capacitor (per post #2)...

In some cases it helps to install a resistor (low ohm) inline with a capacitor.

Or, perhaps a resistor (high ohm) in parallel with the capacitor, particularly when neighboring components are an inductor or diode.

 

[crutschow]

Selecting "Skip Initial Operating Point Solution" (UIC) or "Start external supply voltages at 0V" in the Transient Command should also allow a normal simulation.

 

[schmitt trigger]

It works!

Thanks everyone