# Cannot simulate my model on LTSpice

I'm having trouble trying to simulate my NMOS (FDG6301N) on LTSpice. I have a permanent error telling me

x1:ed: unknown circuit node: "nc_01". requested in behavioral source

I took the model from On semiconductor website.

You can find the model, symbol and part of my schematic here.

The full schematic can be found here.

If you need more data I can post them here.

I'm simulating this NMOS to see its linear behavior. If you know a good NMOS with a huge linear operating range you also can advise me some parts.

• was that model for ltspice or maybe some other spice dialect? – PlasmaHH Jun 4 '18 at 9:21
• You didn't connect the 4th pin, so whatever behavioural source that makes use of that voltage cannot use it. Maybe the solution is to simply add a net, unconnected, or with a label. – a concerned citizen Jun 4 '18 at 9:24
• On the On Semiconductor website it was written as a PSpice model. Is it then only compatible with Orcad software ? – RPerun Jun 4 '18 at 9:25
• @aconcernedcitizen I added a net, not connected to anything and now the Unknown Circuit node is "n005" and no more "nc_01" – RPerun Jun 4 '18 at 9:30
• @RPerun Why not simply post, from the beginning, the whole schematic. Picture might do, for now. The error is telling you that you have a behavioural source which makes use of that node. It was nc_01 (=not connected), now it's n005 (=node), so that must be one half of the problem, you have to know where the behavioural source is. Nobody here will be able to guess unless you post everything you have. Help us help you. The model, as it is, should work in LTspice. – a concerned citizen Jun 4 '18 at 9:34

It looks like, internally, the model has an E-source in the *TEMP section:
ED 101 0 VALUE {V(50,100)}
which is connected to the TEMP pin, and whose expression is, after using the expanded listing:
b:x1:§eout x1:4x x1:6x v=v(x1:1x)*v(x1:3x)
so it multiplies an internal voltage to the external one. That is supplied at the TEMP pin, and comes, most probably, from some thermal design model (heatsink, or similar). If you don't use temperature, then simply ground that pin, else you can supply the temperaure (probably in oC, as Volts, e.g. 58oC = 58V).