Maker Pro
Maker Pro

Spice COMS Invertor?

N

N. Thornton

Jan 1, 1970
0
Hi


I'm looking for a spice model for a CMOS invertor for analogue use. It
needs to reproduce the non linear gain, and the gates' significant
output impedance. It also needs to be run on other than just 5v.

The invertor that comes with LTspice is nothing like this, and is
entirely unsuitable.

I've googled, but found nothing yet. Anyone, anywhere?


NT

PS I've used Spice very little so expect idiot responses :)
 
J

Jim Thompson

Jan 1, 1970
0
Hi


I'm looking for a spice model for a CMOS invertor for analogue use. It
needs to reproduce the non linear gain, and the gates' significant
output impedance. It also needs to be run on other than just 5v.

The invertor that comes with LTspice is nothing like this, and is
entirely unsuitable.

I've googled, but found nothing yet. Anyone, anywhere?


NT

PS I've used Spice very little so expect idiot responses :)

I have the original 'HCU04 stuff (since I redesigned it for ON-Semi).

It may, or may not, work on your simulator, since it relies on a lot
of parameter passing.

What I'd recommend is making your own inverter by pulling generic CMOS
devices from your simulator's library, set width wider until threshold
is mid-supply, and then experiment from there.

...Jim Thompson
 
J

Jim Thompson

Jan 1, 1970
0
I have the original 'HCU04 stuff (since I redesigned it for ON-Semi).

It may, or may not, work on your simulator, since it relies on a lot
of parameter passing.

What I'd recommend is making your own inverter by pulling generic CMOS
devices from your simulator's library, set width wider until threshold
is mid-supply, and then experiment from there.

...Jim Thompson

Make that "...set P-CHANNEL device width wider..."

...Jim Thompson
 
J

Joerg

Jan 1, 1970
0
Hi N. Thornton,

If you are eyeing the unbuffered HC04 version you might be able to
obtain it from a manufacturer. Fairchild offers these. They are not
PSpice but HSpice files so you'd have to parse through by hand. I am not
familiar with HSpice so it may or may not be a big deal to do. Also, I
believe they send them to you "as is" and require you not to divulge it
to other parties and agree to some other conditions. Check it out:

http://www.fairchildsemi.com/models/HSPICE/Interface_and_Logic/HC.html

Regards, Joerg
 
J

Jim Thompson

Jan 1, 1970
0
Hi N. Thornton,

If you are eyeing the unbuffered HC04 version you might be able to
obtain it from a manufacturer. Fairchild offers these. They are not
PSpice but HSpice files so you'd have to parse through by hand. I am not
familiar with HSpice so it may or may not be a big deal to do. Also, I
believe they send them to you "as is" and require you not to divulge it
to other parties and agree to some other conditions. Check it out:

http://www.fairchildsemi.com/models/HSPICE/Interface_and_Logic/HC.html

Regards, Joerg

That's the shits... the model has "protected" (encrypted) device
models, meaning it will only run on HSpice :-(

I guess I'll have to get out my 'HCU04 design and patch all the
oddball "Shrink" and other parameter passing, make it
Spice-flavor-independent and post it.

_Maybe_ this weekend.

...Jim Thompson
 
J

Joerg

Jan 1, 1970
0
Hi Jim,
That's the shits... the model has "protected" (encrypted) device
models, meaning it will only run on HSpice :-(

Maybe the Philips versions (Berkeley Spice) would work and save your
weekend. However, I haven't looked at these myself yet. There are 74HC
but no CD4000 models:

http://www.standardproducts.philips.com/support/spice/#
I guess I'll have to get out my 'HCU04 design and patch all the
oddball "Shrink" and other parameter passing, make it
Spice-flavor-independent and post it.

_Maybe_ this weekend.

But then everyone who uses it and comes through Phoenix later should
treat you for a Widmer's on tap at the local pub :)

Regards, Joerg
 
J

Jim Thompson

Jan 1, 1970
0
Hi Jim,


Maybe the Philips versions (Berkeley Spice) would work and save your
weekend. However, I haven't looked at these myself yet. There are 74HC
but no CD4000 models:

http://www.standardproducts.philips.com/support/spice/#

Those look AOK, except they're LEVEL=3, so a bit lacking for high
speed simulations.
But then everyone who uses it and comes through Phoenix later should
treat you for a Widmer's on tap at the local pub :)

Regards, Joerg

Such a deal ;-)

...Jim Thompson
 
A

Active8

Jan 1, 1970
0
On Wed, 17 Nov 2004 16:28:32 -0700, Jim Thompson wrote:
That's the shits... the model has "protected" (encrypted) device
models, meaning it will only run on HSpice :-(

I guess I'll have to get out my 'HCU04 design and patch all the
oddball "Shrink" and other parameter passing, make it
Spice-flavor-independent and post it.
You know what would really be the balls? A short example of how you
hack your .cir files, pass params, and all that stuff you do to run
worst case. Maybe that first design challenge you issued, if you get
a chance.
 
K

Kevin Aylward

Jan 1, 1970
0
Not sure where this post came from, or if I have already replied or not.
Anyway, as usuall, I have a full complement of analogue versions CMOS
inverters, gates, switches and stuff in my SuperSpice download.

Kevin Aylward
[email protected]
http://www.anasoft.co.uk
SuperSpice, a very affordable Mixed-Mode
Windows Simulator with Schematic Capture,
Waveform Display, FFT's and Filter Design.
 
N

N. Thornton

Jan 1, 1970
0
Jim Thompson said:
On Thu, 18 Nov 2004 01:08:14 GMT, Joerg


Those look AOK, except they're LEVEL=3, so a bit lacking for high
speed simulations.


Such a deal ;-)

...Jim Thompson

Hi again. What I'm actually looking for is 4000 series invertors. I
understood at least some of what you folks said - I really am a spice
cadet when it comes to spice. I used to do paper design and lash up
rather than simulate, and now I want to learn spice and sim a few
ideas, since I intend to get back into tronics again next year. I'm
sure once I've got the hang of it it'll be quicker and more
informative than lashups, not to mention easier. I've got LTspice at
the mo.

Why 4000? Vdd upto 15v, cheap and easily available, and more than fast
enough. 74HC and HCT doesnt do the voltage.

I know LTSPice comes with invertors, but the documentation describes
them as not even a bit suitable, having no modeling of linear gain,
only switching, 0 or 1v out, no output impedance, no ability to alter
supply V, and no nonlinearity. So all in all no use for analogue as
far as I can tell. As far as rewriting its behaviour, I wouldnt have a
clue.


Thanks for trying to clue me up :) NT
 
P

Paul Burridge

Jan 1, 1970
0
I know LTSPice comes with invertors, but the documentation describes
them as not even a bit suitable, having no modeling of linear gain,
only switching, 0 or 1v out, no output impedance, no ability to alter
supply V, and no nonlinearity. So all in all no use for analogue as
far as I can tell. As far as rewriting its behaviour, I wouldnt have a
clue.

I would have thought it would have been a relatively simple matter to
create your own model for something as basic as a gate (even with
fullish operational characteristics). But since you're a Spice virgin,
you'd need someone with a bit of experience to guide you. Helmut
springs to mind...
(I'll cross post to sec and you may like to check out the LTSpice
users' group on Yahoo).
 
E

Emoneg

Jan 1, 1970
0
N. Thornton said:
Hi again. What I'm actually looking for is 4000 series invertors. I
understood at least some of what you folks said - I really am a spice
cadet when it comes to spice. I used to do paper design and lash up
rather than simulate, and now I want to learn spice and sim a few
ideas, since I intend to get back into tronics again next year. I'm
sure once I've got the hang of it it'll be quicker and more
informative than lashups, not to mention easier. I've got LTspice at
the mo.

Why 4000? Vdd upto 15v, cheap and easily available, and more than fast
enough. 74HC and HCT doesnt do the voltage.

I know LTSPice comes with invertors, but the documentation describes
them as not even a bit suitable, having no modeling of linear gain,
only switching, 0 or 1v out, no output impedance, no ability to alter
supply V, and no nonlinearity. So all in all no use for analogue as
far as I can tell. As far as rewriting its behaviour, I wouldnt have a
clue.


Thanks for trying to clue me up :) NT

Google

http://www.google.com/search?hl=en&q=4069UB+spice+model

Link

http://www.abcelectronique.com/simulation_spice/HIFI_LIB.LIB

In Link

*********
..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
SHEET 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
 
J

Jim Thompson

Jan 1, 1970
0
On Wed, 17 Nov 2004 16:28:32 -0700, Jim Thompson wrote:

You know what would really be the balls? A short example of how you
hack your .cir files, pass params, and all that stuff you do to run
worst case. Maybe that first design challenge you issued, if you get
a chance.

Refresh my memory. What was the "first design challenge (I) issued"?

As for worst case, I don't do Monte Carlo, because, in an IC,
components of a given type don't wander relative to each other.

Almost always I am provided (by the foundry) with device libraries
that cover the worst case process corners.

Thus, to do process corner simulations, I just concatenate a bunch of
..CIR files, each with the library/temperature/voltage combination I
want... sometimes as many as 30-40 combinations. PSpice will show all
the outputs on a single screen.... making for nice presentations to
the customer.

...Jim Thompson
 
K

Keith Williams

Jan 1, 1970
0
Refresh my memory. What was the "first design challenge (I) issued"?

As for worst case, I don't do Monte Carlo, because, in an IC,
components of a given type don't wander relative to each other.

Sure they do, with the added complication of device tracking. Monte
Carlo is used quite heavily in IC design.
Almost always I am provided (by the foundry) with device libraries
that cover the worst case process corners.

Sure, but end-point analysis just cuts down on CPU cycles. ;-) I've
used both at the same time (end-point distributions chugged into Monte
Carlo analysis).
Thus, to do process corner simulations, I just concatenate a bunch of
.CIR files, each with the library/temperature/voltage combination I
want... sometimes as many as 30-40 combinations. PSpice will show all
the outputs on a single screen.... making for nice presentations to
the customer.

That's not much different than the above (Monte Carlo using worst-case
numbers).
 
J

Jim Thompson

Jan 1, 1970
0
[email protected] says... [snip]
As for worst case, I don't do Monte Carlo, because, in an IC,
components of a given type don't wander relative to each other.

Sure they do, with the added complication of device tracking.

Device tracking problems are only an issue with amateur designers ;-)
Monte
Carlo is used quite heavily in IC design.


Sure, but end-point analysis just cuts down on CPU cycles. ;-) I've
used both at the same time (end-point distributions chugged into Monte
Carlo analysis).


That's not much different than the above (Monte Carlo using worst-case
numbers).

In all my years in IC design I have seen ONLY ONE foundry that
provided models with Monte-Carlo-specified parameters, and that was
from a village-idiot foundry that took their GUESSED-AT models and
added deviations ;-)

...Jim Thompson
 
J

Joerg

Jan 1, 1970
0
Hi Jim,
Thus, to do process corner simulations, I just concatenate a bunch of
.CIR files, each with the library/temperature/voltage combination I
want... sometimes as many as 30-40 combinations. PSpice will show all
the outputs on a single screen.... making for nice presentations to
the customer.

30-40 on one slide, that's a lot. Just make sure that nobody in the
audience is color blind. Seriously, I had that happen a couple of times.
And the "morse code pattern" only goes so far for folks sitting in the
back rows.

Regards, Joerg
 
J

Jim Thompson

Jan 1, 1970
0
Hi Jim,


30-40 on one slide, that's a lot. Just make sure that nobody in the
audience is color blind. Seriously, I had that happen a couple of times.
And the "morse code pattern" only goes so far for folks sitting in the
back rows.

Regards, Joerg

I have created some "parts" in PSpice which display the spec bounds in
PROBE. Thus it's easy to see the "bundle" of waveforms fitting inside
the bounds, even though it's a swirly mess of colored traces ;-)

...Jim Thompson
 
K

Keith Williams

Jan 1, 1970
0
[email protected] says... [snip]
As for worst case, I don't do Monte Carlo, because, in an IC,
components of a given type don't wander relative to each other.

Sure they do, with the added complication of device tracking.

Device tracking problems are only an issue with amateur designers ;-)

Tracking problems don't exist? You must live in a charmed world of
perfection. However, I must say that I no longer do circuit design,
so... ;-)
In all my years in IC design I have seen ONLY ONE foundry that
provided models with Monte-Carlo-specified parameters, and that was
from a village-idiot foundry that took their GUESSED-AT models and
added deviations ;-)

All the models I've seen have parameters useful for such simulation and
I suppose I've called our foundry folks worse things. ;-0
 
J

Jim Thompson

Jan 1, 1970
0
[email protected] says... [snip]

As for worst case, I don't do Monte Carlo, because, in an IC,
components of a given type don't wander relative to each other.

Sure they do, with the added complication of device tracking.

Device tracking problems are only an issue with amateur designers ;-)

Tracking problems don't exist? You must live in a charmed world of
perfection. However, I must say that I no longer do circuit design,
so... ;-)

Devices that are located a few microns apart DO tend to track...
designers who rely on tracking cross-chip are fools ;-)
All the models I've seen have parameters useful for such simulation and
I suppose I've called our foundry folks worse things. ;-0

Sure. I get pages and pages of parameters, but they're not
Monte-Carlo-based, they're parameter passing for the specific library
corner. For example:

***************** CORNER_LIB OF TNTP MODEL ***************
*.LIB TT_33
..param
+toxn_33 = 7.15E-09 toxp_33 = 7.15E-09
+dvthn_33 = 0 dvthp_33 = 0
+dwvthn_33 = 0 dwvthp_33 = 0
+dxl_33 = 0 dxw_33 = 0
+cjn_33 = 0.00091 cjp_33 = 0.001267
+cjswn_33 = 1.180E-10 cjswp_33 = 0.740E-10
+cjswgn_33 = 2.310E-10 cjswgp_33 = 1.590E-10
+cgon_33 = 2.920E-10 cgop_33 = 2.440E-10
+hdifn_33 = 1.30E-07 hdifp_33 = 1.30E-07
*.ENDL TT_33
**********************************************************
..LIB C:\PSpice\DeviceLib\SomeFAB\CurrentModels\CMOSdoodah.lib
**********************************************************
..PARAM XLN = {0+dxl_33} XWN = {1E-8+dxw_33}
+ XLP = {5E-9+dxl_33} XWP = {1E-8+dxw_33}
**********************************************************

...Jim Thompson
 
K

Keith Williams

Jan 1, 1970
0
[snip]

As for worst case, I don't do Monte Carlo, because, in an IC,
components of a given type don't wander relative to each other.

Sure they do, with the added complication of device tracking.

Device tracking problems are only an issue with amateur designers ;-)

Tracking problems don't exist? You must live in a charmed world of
perfection. However, I must say that I no longer do circuit design,
so... ;-)

Devices that are located a few microns apart DO tend to track...
designers who rely on tracking cross-chip are fools ;-)

Devices across chip *tend* to track too, just not as well as those next
door. It's all a matter of degree. Nothing is perfect. I always
modeled tracking even with "identical" devices right next door. I
suppose it depends on how good the models are, whether the difference
is apparent.
Sure. I get pages and pages of parameters, but they're not
Monte-Carlo-based, they're parameter passing for the specific library
corner. For example:

***************** CORNER_LIB OF TNTP MODEL ***************
*.LIB TT_33
.param
+toxn_33 = 7.15E-09 toxp_33 = 7.15E-09
+dvthn_33 = 0 dvthp_33 = 0
+dwvthn_33 = 0 dwvthp_33 = 0
+dxl_33 = 0 dxw_33 = 0
+cjn_33 = 0.00091 cjp_33 = 0.001267
+cjswn_33 = 1.180E-10 cjswp_33 = 0.740E-10
+cjswgn_33 = 2.310E-10 cjswgp_33 = 1.590E-10
+cgon_33 = 2.920E-10 cgop_33 = 2.440E-10
+hdifn_33 = 1.30E-07 hdifp_33 = 1.30E-07
*.ENDL TT_33
**********************************************************
.LIB C:\PSpice\DeviceLib\SomeFAB\CurrentModels\CMOSdoodah.lib
**********************************************************
.PARAM XLN = {0+dxl_33} XWN = {1E-8+dxw_33}
+ XLP = {5E-9+dxl_33} XWP = {1E-8+dxw_33}
**********************************************************

The models I've used have the distribution specified (mean and sigma,
at least, if not a distribution function). Indeed one can specify
where within the process one wants to run. Want to center at +3sigma?
Go fer it, here's the bill. ;-)

Again, it's been a while since I've actually done circuit design (and
that was bipolar), but I haven't noticed the world change too much.
Perhaps I'll wander off and bug a circuit designer if I get a few
minutes before everyone (me included;) leaves for the holiday.
 
Top