Re: 4069 as an amplifier spice model?

From: Helmut Sennewald (helmutsennewald_at_t-online.de)
Date: 12/23/04 

Date: Thu, 23 Dec 2004 01:52:46 +0100

"Malcolm Reeves" <mreeves@fullcircuit.com> schrieb im Newsbeitrag
news:qsrjs0tdjk674jsr3228p85ok5olfqmn9i@4ax.com...
> Hi,
>
> Anyone know of a spice model for a 4069 buffer being used as an
> amplifier? If there is one in pspice I can't find it.
>
> Or come to that, info on what the params for a 4069 used as an
> amplifier are.
>

Hello Malcolm,
there has been a similar question in sci.electronics.design
in November(11/18/2004). The original postings are attached.

.SUBCKT 4069UB 6 1 4
*Connections e s Vcc
M2 1 6 0 0 CD4069BN
M3 1 6 4 4 CD4069BP
.MODEL CD4069BN NMOS (LEVEL=1 VTO=2.1 KP=2.9M GAMMA=3.97U
+ PHI=.75 LAMBDA=1.87M RD=20.2 RS=184.1 IS=31.2F PB=.8 MJ=.46
+ CBD=47.6P CBS=57.2P CGSO=70.2N CGDO=58.5N CGBO=96.3N)
.MODEL CD4069BP PMOS (LEVEL=1 VTO=-2.9 KP=2M GAMMA=3.97U
+ PHI=.75 LAMBDA=1.87M RD=28.2 RS=145.2 IS=31.2F PB=.8 MJ=.46
+ CBD=47.6P CBS=57.2P CGSO=70.2N CGDO=58.5N CGBO=96.3N)
.ENDS 4069UB

Best Rgeards,
Helmut

--- Original thread from sci.electronics.design ---

"N. Thornton" <bigcat@meeow.co.uk> wrote in message
news:a7076635.0411181739.535b62a4@posting.google.com...
> "Emoneg" <and@nothere.net> wrote in message
news:<ix2nd.53$6q3.41@newsfe6-win.ntli.net>...
>
> > *********
> > .SUBCKT 4069UB 6 1 4
> > *Connections e s Vcc
> > M2 1 6 0 0 CD4069BN
> > M3 1 6 4 4 CD4069BP
> > .MODEL CD4069BN NMOS (LEVEL=1 VTO=2.1 KP=2.9M GAMMA=3.97U
> > + PHI=.75 LAMBDA=1.87M RD=20.2 RS=184.1 IS=31.2F PB=.8 MJ=.46
> > + CBD=47.6P CBS=57.2P CGSO=70.2N CGDO=58.5N CGBO=96.3N)
> > .MODEL CD4069BP PMOS (LEVEL=1 VTO=-2.9 KP=2M GAMMA=3.97U
> > + PHI=.75 LAMBDA=1.87M RD=28.2 RS=145.2 IS=31.2F PB=.8 MJ=.46
> > + CBD=47.6P CBS=57.2P CGSO=70.2N CGDO=58.5N CGBO=96.3N)
> > .ENDS 4069UB
> > *$
> > *
> > *************
> >
> > In LTSPICE
> >
> > Version 4
> > *** 1 1240 680
> > WIRE 144 160 96 160
> > WIRE 96 160 96 288
> > WIRE 96 432 144 432
> > WIRE 192 352 192 288
> > WIRE 192 144 192 112
> > WIRE 192 448 192 480
> > WIRE 96 288 48 288
> > WIRE 96 288 96 432
> > WIRE 192 288 240 288
> > WIRE 192 288 192 240
> > FLAG 192 112 VDD
> > IOPIN 192 112 In
> > FLAG 192 480 VDD
> > IOPIN 192 480 In
> > FLAG 48 288 IN
> > IOPIN 48 288 In
> > FLAG 240 288 OUT
> > IOPIN 240 288 Out
> > SYMBOL nmos 144 352 R0
> > WINDOW 0 57 39 Left 0
> > WINDOW 3 58 60 Left 0
> > SYMATTR InstName M2
> > SYMATTR Value CD4069BN
> > SYMBOL pmos 144 240 M180
> > WINDOW 0 60 59 Left 0
> > WINDOW 3 59 34 Left 0
> > SYMATTR InstName M1
> > SYMATTR Value CD4069BP
> > TEXT 336 232 Left 0 !.MODEL CD4069BN NMOS (LEVEL=1 VTO=2.1 KP=2.9M
> > GAMMA=3.97U\n+ PHI=.75 LAMBDA=1.87M RD=20.2 RS=184.1 IS=31.2F PB=.8
> > MJ=.46\n+ CBD=47.6P CBS=57.2P CGSO=70.2N CGDO=58.5N CGBO=96.3N)\n.MODEL
> > CD4069BP PMOS (LEVEL=1 VTO=-2.9 KP=2M GAMMA=3.97U\n+ PHI=.75
LAMBDA=1.87M
> > RD=28.2 RS=145.2 IS=31.2F PB=.8 MJ=.46\n+ CBD=47.6P CBS=57.2P CGSO=70.2N
> > CGDO=58.5N CGBO=96.3N)
> >
> >
> > OK, it's a bit of a hack but someone else might tidy it up.
> >
> > DNA
>
> Aha! Looks promising... now what do I do with that bit of text to make
> a component model with it? I'm putting the circuit in using circuit
> piccies, not using a netlist.
>
> Thanks, NT

You copy the text into notepad and then save the file with a .asc extension.
LTspice will then open it up as a schematic.

DNA