Hello all,
I’m trying to import the Spice model for an FQP27P06 MOSFET, but it fails to load due to the phrase: “…FQP27P06.lib:8:51: expected”. I’ve attached a screenshot and also the model file. Might “8:51” refer to a line number in the file containing the error, or possibly an error code?
I would appreciate anyone’s help very much!
FQP27P06.txt (1.5 KB)
It refers to line 8 character 51. The kicad parser has trouble with the formula there. I think you can fix that by factoring out the formula and replacing the curly braces. I had to do something like that before so kicad would swallow the model:
.SUBCKT FQP27P06 20 10 30
Rg 10 1 1.58
M1 2 1 3 3 DMOS L=1u W=1u
.MODEL DMOS PMOS(VTO=(0.002976*TEMP-3.1744) KP=(-0.0068*TEMP+10.4)
+ THETA=0.0576 VMAX=3.0E5 ETA=0.004 LEVEL=3)
Cgs 1 3 990p
Rd 20 4 0.018 TC=0.0055
Dds 4 3 DDS
.MODEL DDS D(BV=(0.05849*TEMP+58.5374) M=0.44 CJO=1380p VJ=0.76)
...
Please double check what I calculated there, this is very rough. If you don’t care about the temperature, you can also set that to a fixed temperature and just calculate the values for VTO and KP and BV. Maybe someone who understands more about the model can give you some more insides. I believe this might be entirely a KiCad problem and not have anything to do with ngspice. KiCad parses the model on its side when assigning a model. Maybe I will try tomorrow if ngspice would handle this model without modification, but it is getting kind of late here …
Nested curly braces are rejected by KiCad/Eeschema. ngspice should have no problems with these. Some time ago I have made an update to ngspice to replace the inner curly braces by round brackets (automatically during parsing the model file).
I checked this with ngspice earlier and ngspice handles the model gracefully (if pspice compatibility is set with set ngbehavior=ltps ). I am kind of wondering why KiCad needs to parse the spice model to the extend that it does.
This topic was automatically closed after 90 days. New replies are no longer allowed.