2
\$\begingroup\$

Hello I get errors with MOSFET spice models from Nexperia,

I've tried to include the spice fil within the asc and as .include to the lib, the error is the same. I think it may be so that the spice syntax in the model is not correct for LTspice, lambda seem to be a real variable for LTspice so on that one I don't understand why it complains. enter image description here

Link to: Mosfet in question

I get the following error

Error on line 45 : .model m1:psmn017_80ps.lib nmos(vto=4.04250999509733 kp=1.5055e+02 nfs=0 eta=0 level=3 l=1e-4 w=1e-4 gamma=0 phi=0.6 lambda=0 is=1e-24 js=0 pb=0.8 pbsw=0.8 vmax=1000) * Unrecognized parameter "lambda" -- ignored Error on line 45 : .model m1:psmn017_80ps.lib nmos(vto=4.04250999509733 kp=1.5055e+02 nfs=0 eta=0 level=3 l=1e-4 w=1e-4 gamma=0 phi=0.6 lambda=0 is=1e-24 js=0 pb=0.8 pbsw=0.8 vmax=1000) * Unrecognized parameter "pbsw" -- ignored

Any ideas on how to fix this?

\$\endgroup\$

1 Answer 1

6
\$\begingroup\$

The problem looks to be due to this .model statement:

.MODEL MINT NMOS(Vto=4.04250999509733 Kp=1.5055e+02 Nfs=0 Eta=0
+ Level=3 L=1e-4 W=1e-4 Gamma=0 Phi=0.6 Lambda=0 Is=1e-24
+ Js=0 Pb=0.8 Pbsw=0.8 Vmax=1000)

There are a couple ways to fix it. The most straightforward is to delete Lambda=0 and Pbsw=0.8. It should look like this after you do that:

.MODEL MINT NMOS(Vto=4.04250999509733 Kp=1.5055e+02 Nfs=0 Eta=0
+ Level=3 L=1e-4 W=1e-4 Gamma=0 Phi=0.6 Is=1e-24
+ Js=0 Pb=0.8 Vmax=1000)

The justification for this is that Lambda is not supposed to be used with Level=3 models, which is an error by whomever created the model. Pbsw is the sidewall junction potential which LTspice doesn't use, which is fine because Pb (the bottom junction potential) is defined and at the same potential of 0.8.

\$\endgroup\$

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.