|
Hi Tony,
?
Thanks for providing this case. In a nicely condensed form, it demonstrates the problems of legacy LTspice and how they are addressed by 24.1.
You have two models:
?
.model 0 AKO: BSP89
.model 1 AKO: BSS145 ?
and the line
?
M1 D G 0 0 {M}
?
Legacy LTspice (aka the version that you assumed "works") interprets the the second "0" as the model name. That's because there is a model with the name "0" defined. However, the actual intent for this "0" is to label the substrate node. (As documented in the help.) It then goes on and finds "{M}" which resolves to "0". This is interpreted as a parameter to M1, but a single "0" is not a valid parameter. It keeps going, at the end you get a visible error message in the log:
?
Error on line 4 : m1 d g 0 0 ?0?
? ? Error: ?No unlabeled parameter permitted for MOSFET's ?
If you changed the M1 line into:
?
M1 D G 0 1 {M}
?
you'd expect the substrate node to be connected to node "1" and model "{M}" be used. Instead, legacy LTspice will use model "1" and again ignore "{M}" as invalid parameter. Still, it keeps going.
?
LTspice 24.1 behaves in exactly the same way, except that it aborts with a hard error and a much better error message. This is the only acceptable behavior, because there is no point running a sim that obviously doesn't work out as the user intended.
?
All this boils down to the fact that the spice netlist format is poorly designed.
?
LTspice 24.1 introduces string parameters and thereby eliminates the need to name models like numbers, thus greatly reducing the likelihood of problems.
?
Best Regards,
Mathias
?
?
On Tue, Mar 4, 2025 at 11:38 AM, Tony Casey wrote:
I have uploaded an example schematic that shows 3 options for stepping MOSFET models: Stepping_Models_pre-V24.1_workaround. Option 1: works only in 24.1 |
