On Fri, Apr 11, 2025 at 05:15 PM, Richard Andrews wrote:
This is how it should be done, but I got a warning in the log file using version 4.
Your schematic has two things wrong.? This is not how it should be done.
- You defined a diode model with a name that already exists.? MUR460 is in standard.dio, in LTspice's diode library.? Don't try overriding a model that was already defined.? Aside from the warning, you don't know for sure which model definition it ends up using.? Better to use a name like "MyMUR460" or "JUNK".
- You altered the wrong "N".
?
As I discussed already (
perhaps you missed it), the "N" that is inside a diode's .MODEL definition is not the same as the "N" that goes on the diode's element line.
?
"N" inside a diode's .MODEL definition is the diode's "Emission Coefficient".? It is the same "n" that is in the Shockley Ideal Diode Law, multiplied by (kT/q) and in the denominator of the exponent of "e".? Its normal value is 1.0, and can be set a little larger, usually between 1 and 2, to indicate a "less perfect" diode.? That is its intended purpose.? Some SPICE models set N unusually low, apparently to construct a theoretical diode with much less than the normal forward voltage.
?
"N" when used in the diode element line sets the number of effective diodes connected in series.? N=5 means this one diode in your schematic represents 5 diodes in series.? It can have fractional values too, such as 5.31.
?
The two N's must never be confused!? They are two completely different things.
?
In this example, Dave wanted to use the "N" diode multiplier, which must be part of the diode element line and must not be inside the diode's .MODEL statement.? But "Rs" is a .MODEL parameter so it must be inside the diode's .MODEL statement.
?
Andy
?
