SPICE model for 4538 monostable ?

[jmelson]

Anybody know where to get a generic SPICE model for a 4538 monostable?

There is a HIDEOUS file from TI that has about 100 parts in it, but they are all just I/O models, with no actual logic function inside.  The late Jim Thompson apparently created a model, but I can't find the actual file, his web site seems to have gone down sometime after his demise.

I want to simulate something so I make sure I have the right connections to the positive- and negative-triggered edge inputs.

Thanks for any help,

Jon

[Wimberleytech]

Found this on github

* (DUAL) RETRIGGERABLE MONOSTABLE MULTIVIBRATOR
* Pulse Width Tw = 0.7 * R * C
* tpd R,A,B->Q     30n
* Tpulse 75n, C=0, Rext=5k
.SUBCKT 74HC4538  A B CLR  CGND RC  Q QN  VCC VGND  vcc1={vcc} speed1={speed} tripdt1={tripdt}
.param egain=1/{vcc1}
.param td5=1e-9*(5)*4.0/({vcc1}-0.5)*{speed1}
.param td2=1e-9*(2)*4.0/({vcc1}-0.5)*{speed1}
*
XINA    A Ai  VCC VGND  74HC_IN_1  vcc2={vcc1}  speed2={speed1}  tripdt2={tripdt1}
XINB    B Bi  VCC VGND  74HC_IN_1  vcc2={vcc1}  speed2={speed1}  tripdt2={tripdt1}
XINCLR  CLR CLRi  VCC VGND  74HC_IN_1  vcc2={vcc1}  speed2={speed1}  tripdt2={tripdt1}
XINRC1  RC RCi  VCC VGND  74HC_IN_0  vcc2={vcc1}  speed2={speed1}  tripdt2={tripdt1}
*
* Model of a 74HC123A derived  from SGS-Thomson data sheet.
* Helmut Sennewald, 13.9.2002
A4 DHIGH 0 N014 0 N004 N006 N005 0 DFLOP   tripdt={tripdt1}  td={td5}
*A3 0 N015 N016 N023 0  N014 0 0 OR  tripdt={tripdt1}  td={td5}
A3 0 N015 N016 0 0     0 N014 0  OR  tripdt={tripdt1}  td={td5}
A1 Ai 0 0 0 0          0 N015 0  SCHMITT  Vt=0.46 Vh=0.02  tripdt={tripdt1}  td={td5}
A2 Bi 0 0 0 0          N016 0 0  SCHMITT  Vt=0.46 Vh=0.02  tripdt={tripdt1}  td={td5}
A6 0 N008 0 N006 0     N007 0 0  AND  tripdt={tripdt1}  td={td5}
A5 0 N009 0 N007 0     N008 0 0  AND  tripdt={tripdt1}  td={td5}
A14 0 N003 0 N021 0    N004 0 0  AND  tripdt={tripdt1}  td={td2}
A13 0 N003 0 N005 0    0 N030 0  AND  tripdt={tripdt1}  td={td5}
A12 N005 0 0 0 0       N012 0 0  BUF  tripdt={tripdt1}  td={td5}
A21 0 N010 0 N011 0    0 N009 0  OR  tripdt={tripdt1}  td={td5}
A22 0 N005 0 N007 0    N010 0 0  OR  tripdt={tripdt1}  td={td5}
A11 0 N013 0 N012 0    0 N003 0  OR  tripdt={tripdt1}  td={td5}
A7 0 N007 0 N018 0     QNi Qi 0  AND  tripdt={tripdt1}  td={td5}
A20 RCi 0 0 0 0        N011 0 0  SCHMITT  tripdt={tripdt1}  td={td5}  Vt=0.54 Vh=0.2m
A10 RCi 0 0 0 0        0 N013 0  SCHMITT  tripdt={tripdt1}  td={td5}  Vt=0.1 Vh=0.2m
A32 0 N006 0 N021 0    N022 0 0  OR  tripdt={tripdt1}  td={td5}
A31 0 N022 0 N023 0    N021 0 0  OR  tripdt={tripdt1}  td={td2}
A33 N021 0 0 0 0       N019 0 0  BUF  tripdt={tripdt1}  td={td5}
A30 CLRi 0 0 0 0       N023 0 0  BUF  tripdt={tripdt1}  td={td5}
A34 0 N007 0 N006 0    N020 0 0  AND  tripdt={tripdt1}  td={td5}
A35 0 N020 0 N018 0    N017 0 0  OR  tripdt={tripdt1}  td={td5}
A36 0 N017 0 N019 0    N018 0 0  OR  tripdt={tripdt1}  td={td5}
M10 RC N001 VGND VGND NMOS1
M30 RC N024 VCC VCC PMOS1
D1 RC VCC DIO1
D2 VGND RC DIO1
R10 N001 N002 100
R30 N024 N029 100
R3 CGND VGND 1
E4 RCi 0 RC VGND {egain}
E7 N029 VCC N018 0 {vcc1}
E8 N002 VGND N030 0 {vcc1}
V1 DHIGH 0 DC 1
.MODEL NMOS1 NMOS ( LEVEL=3  W=500e-6  L=1E-6  VTO=1
+ VMAX=1E6  RS=10  RD=10  CJ=0.002  MJ=0.4
+THETA=1E-6 ETA=0.01  KAPPA=2.2)
.MODEL PMOS1 PMOS ( LEVEL=3  W=500e-6  L=1E-6  VTO=-1
+ VMAX=1E6  RS=10  RD=10  CJ=0.002  MJ=0.4
+THETA=1E-6 ETA=0.01  KAPPA=2.2)
.MODEL DIO1 D (IS=10p RS=10 N=1.75 M=0.4 Cjo=6p TT=20n)
*
XOUT0  Qi  Q   VCC VGND  74HC_OUT_1X  vcc2={vcc1} speed2={speed1}  tripdt2={tripdt1}
XOUT1  QNi QN  VCC VGND  74HC_OUT_1X  vcc2={vcc1} speed2={speed1}  tripdt2={tripdt1}
.ends

[RomDump]

The late Jim Thompson apparently created a model, but I can't find the actual file, his web site seems to have gone down sometime after his demise.

Jim Thompson Model

[jmelson]

Thanks very much, guys!

Jon

[jmelson]

Ugh, thanks were  a bit too soon.  The first one was incomplete, it calls in a bunch of I/O subcircuits like 74HC_IN_1, which are not included.

And, the Jim Thompson one, although it says "run on ANY simulator" has a lot of syntax that is not compatible with my sim (basic SPICE included in Protel 99SE).  So, there are things like :
E_E6 N_1 GND VALUE { V(Rbar, GND)/V(VCC) }

I converted these to :

E_E6 N_1 GND VOL='V(Rbar, GND)/V(VCC)'

which seemed to satisfy the syntax, but I get a page of errors when I try to run the simulation.

Anybody recognize the flavor of SPICE this was written in?


Thanks,

Jon

[Wimberleytech]

Here is the github link from where I grabbed the post above.  It prolly has those other subckts

https://github.com/texane/power_inverter/blob/master/ltspice/logic/74hc/74hc.lib

[RomDump]

Anybody recognize the flavor of SPICE this was written in?

Jim use to write his models for PSpice. However, looking at the files in the archive it looks like it is for LTSpice (Which you can download for free and use).