Erros simulating netlist with subckt

[analog_match]

I am trying to run a simple simulation using a call to a subckt. My netlist is below:

X1 Drn Gate gnd gnd nmos1 n=3 m=2 l=2u fw=3u
R1 Drn Drn1 1.0
.subckt nmos1 D G S B n=1 m=1 l=2u fw=2u
.param W={fw*n}
.param L={l}
.param m={m}
M1 D G S B NM m L W
.MODEL NM NMOS VTO=1.0
.ends nmos1

But when I run a sim in ngspice I get the following message:

ngspice 191 -> source test_nmos2.spi

Circuit: *** spice deck for cell test_nmos{sch} from library testgpdk

Error on line 0 : m.x1.m1 drn gate 0 0 x1.nm x1.m l    9.000000000e-06
Unable to find definition of model x1.nm - default assumed

unknown parameter (x1.m)

1.Why is ngspice concatenating the subckt name x1 in front of the subckt call?
2.From the error message, the

.param W={n*fw}

seems to have evaluated correctly to 9u. This is even more puzzling. Why is one parameter evaluating correctly but model name is not being resolved?

Just for comparison I have another netlist that has a subckt call that works. It is as follows:

xyres_yres3@0 vin vout yres
+W=5u
+L=5u
xyres_yres3@1 vout gnd yres
+W=5u
+L=10u
.subckt yres PLUS MINUS W=3u L=3u
.param sheetrho=100.0
.param rval={sheetrho*L/W}
r0 PLUS MINUS rval TC1=0.002
.ends yres

The major difference between the two is that the second one that works does not have a .model statement. Could defining a .model somehow be causing the issue?

Is there a problem with my syntax or is this a bug ?

[Holger Vogt]

There is a bug in your input file.

If you look at the manual, chapt. 11.1, you see the syntax for a MOSFET:
MXXXXXXX nd ng ns nb mname <m=val > < l =val > <w=val >
+ <ad=val > <as=val > <pd=val > <ps=val > <nrd=val >
+ <nrs=val > <of f > < i c =vds , vgs , vbs> <temp=t >

Your MOSFET line has to read
M1 D G S B NM m=m L=L W=W

Holger

[analog_match]

Thank you Holger. Your suggestion solved my issue. Your help is much appreciated.