¿ªÔÆÌåÓý

  1. LTspice
  2. Messages
Expanded Topics Messages Polls
Date
Re: Suggestions for waveform viewer

Arnold Esper
 

An: "'LTspice@...'" <LTspice@...>

Von: "Schaich, Peter" <schaich.peter@...>
Datum: Wed, 26 Mar 2003 08:01:58 +0100
Betreff:[LTspice] Suggestions for waveform viewer



> Hi there,
>
>
> LTSpice is really fun to work with. Assuming that Mike likes to get
> feedback, I would like to make some suggestions for enhancements of the
> waveform viewer, mainly for documentation purposes:
>
> * If any parameter of the circuit is stepped with the .step command, it
> should be possible in the waveform viewer to see what value the parameter
> has in the respective curve. (see example stempodelparam.asc) Preferably
> on a legend that can be switched on or off.
>
> * the number of the cursor should always be displayed, not only on
> mouseover.
>
> * maybe it should be possible to add some draw elements for documentation
>
> * add a second color profile for the use of the results (via clipboard
> copy) in other documents with white background and different colors for
> grid, cursors and axis (cursor color is currently not customizable). There
> is no doubt that black background is good for working on the screen but
> white background is good for documentation.
>
> What are your thoughts?
>
> Regards
>
> Peter Schaich
Yes, it's a good Idea to allow white background to the graphik Window, in order
to save printing-color or some extra work for inverting it for other programs.
The black background reminds me my analog oszilloscope, earlier used every day.
But nowadays I'm almost afraid to touch it's knobs, because of the huge dust on
it.
Maybe a good Idea too, to allow some differnt styles of drawing lines like
dotted, hatched .... for black and white coying machines. Adding the unit behind
every number can make it difficult to read at high line-densities. The Windows
could have a look similar to the picture below, I made with an early Version of
Spice2.
.
Thanks, Arnold
Re: dflops?

David Pariseau
 

Mike,

There's some special things you need to know
about the gates. The gates don't need external
power. If you want a gate to switch between
0 and 5 volts, give the gate a value of
"Vhigh=5" Vlow defaults to 0V.
I figured it was something like this. How do I
set Vhigh=5 for a particular gate??? I was looking
for something like this. It would have to be in a
particular instance right, not at the component level.

Also, all unconnected inputs are connected to
the gate's common node(that extra pin that is
tied to ground in the examples).
Fair enough, that makes things easier. Are the
PRE and CLR inputs active high? Can you tell this
by looking at the component? I wasn't able to find
any documentation on the flip-flop via help, etc...

Thanks for the help,
Dave Pariseau.
Re: dflops?

 

David,

I'm trying to use the dflop part in a simple
circuit and am having difficulty getting it
to work.

+-----------+
0-6v square wave --------|>CLK Q |--- 1v solid
out??
GND----| D Q'|
+-----------+

Both the CLR and the PRE inputs are floating
though I've tried tieing them up and down.

There doesn't seem to be anywhere to attach
power to the device? There is a common pin
(COM?) on the corner, but leaving it open or
tieing it to ground has the same effect.

I'm looking for a 5-6v output. The 160 example
has dflops in it and seems to work fine, which
is beyond me.

Any ideas?
There's some special things you need to know
about the gates.

The gates don't need external power. If you
want a gate to switch between 0 and 5 volts,
give the gate a value of "Vhigh=5" Vlow
defaults to 0V.

Also, all unconnected inputs are connected to
the gate's common node(that extra pin that is
tied to ground in the examples). This
connection flags that pin as unused and is
removed from the simulation. Note that the
common pin will be connected to ground by the
netlister if it is left floating. So, say you
place an AND gate on the schematic, connect one
of it's input to a signal, one input to ground
and leave the other 3 inputs floating. The
AND's output will follow the signal because
all the other pins aren't floating or grounded,
but flagged as not part of the simulation.

--Mike

__________________________________________________
Do you Yahoo!?
Yahoo! Platinum - Watch CBS' NCAA March Madness, live on your desktop!
dflops?

David Pariseau
 

I'm trying to use the dflop part in a simple
circuit and am having difficulty getting it
to work.

+-----------+
0-6v square wave --------|>CLK Q |--- 1v solid out??
GND----| D Q'|
+-----------+

Both the CLR and the PRE inputs are floating
though I've tried tieing them up and down.

There doesn't seem to be anywhere to attach
power to the device? There is a common pin
(COM?) on the corner, but leaving it open or
tieing it to ground has the same effect.

I'm looking for a 5-6v output. The 160 example
has dflops in it and seems to work fine, which
is beyond me.

Any ideas?
Thanks,
David Pariseau.
Re: New Feature Released & Opamp Modeling

 

Jon,

...For example, if I select 2N6028 in the drop-down
for SpiceModel *and* then manually change the Value
attribute to match, everything works well...
You probably want to make the Model and Instance name
visible in the .asy file and nothing else. THE VALUE
SHOULD BE LEFT BLANK in both the .asy and instance,
unless you want to add parameters to pass to the
subckt. These should be of the form "eta=5.3"

Attached is a .asy file and .sub file that work
together
to demonstate being able to use the drop list to
to select a subckt in the .sub file. You will have
to fix line wrap.

--- .asy ---
Version 4
SymbolType CELL
LINE Normal -32 -32 32 0
LINE Normal -32 32 32 0
LINE Normal -32 -32 -32 32
LINE Normal -28 -16 -20 -16
LINE Normal -28 16 -20 16
LINE Normal -24 20 -24 12
LINE Normal 0 -32 0 -16
LINE Normal 0 32 0 16
LINE Normal 4 -20 12 -20
LINE Normal 8 -24 8 -16
LINE Normal 4 20 12 20
WINDOW 0 16 -32 Left 0
WINDOW 38 47 28 Center 0
SYMATTR Prefix X
SYMATTR Description Parameterized Single Pole Opamp.
En and in are equivalent voltage and current noises.
Enk and ink are the respective corner frequencies.
SYMATTR Value2 Avol=10Meg GBW=10Meg Slew=10Meg
SYMATTR SpiceLine ilimit=25m rail=0 Vos=0
SYMATTR SpiceLine2 en=0 enk=0 in=0 ink=0
SYMATTR ModelFile genopamp.sub
SYMATTR SpiceModel 1pole
PIN -32 16 NONE 0
PINATTR PinName In+
PINATTR SpiceOrder 1
PIN -32 -16 NONE 0
PINATTR PinName In-
PINATTR SpiceOrder 2
PIN 0 -32 NONE 0
PINATTR PinName V+
PINATTR SpiceOrder 3
PIN 0 32 NONE 0
PINATTR PinName V-
PINATTR SpiceOrder 4
PIN 32 0 NONE 0
PINATTR PinName OUT
PINATTR SpiceOrder 5

--- .sub ---
* Copyright Linear Technology Corp. 1998, 1999,
2000, 2001, 2002, 2003. All rights reserved.
*
.subckt 1pole 1 2 3 4 5
S1 5 3 N002 5 Q
S2 4 5 5 N002 Q
A1 2 1 0 0 0 0 N002 0 OTA G={Avol/Rout} ref={Vos}
Iout={slew*Cout} Cout={Cout} en={en} enk={enk} in={in}
ink={ink} Vhigh=1e308 Vlow=-1e308
C3 5 4 1p
C4 3 5 1p
S3 N002 0 4 N002 C
S4 0 N002 N002 3 C
R2 N002 4 {2*Rout} noiseless
R1 3 N002 {2*Rout} noiseless
R3 3 1 1G noiseless
R4 3 2 1G noiseless
R5 2 4 1G noiseless
R6 1 4 1G noiseless
.model C SW(Ron=100 Roff=1T Vt=0 Vh=-1 noiseless)
.param Rout=100Meg
.param Cout={Avol/GBW/2/pi/Rout}
.model Q SW(Ron=10 Roff=10Meg Vt=0 Vh=-.1 Vser={Rail}
ilimit={Ilimit} noiseless)
.param Avol=10Meg GBW=10Meg Slew=10Meg ilimit=25m
rail=0 Vos=0
.param en=0 enk=0 in=0 ink=0
.ends 1pole

.subckt 2pole 1 2 3 4 5
S1 5 3 N002 5 Q
S2 4 5 5 N002 Q
A1 2 1 0 0 0 0 N003 0 OTA G={Avol/Rout} ref={Vos}
Iout={slew*Cout} Cout={Cout} en={en} enk={enk} in={in}
ink={ink} Vhigh=1e308 Vlow=-1e308 Rout={Rout}
C3 5 4 1p
C4 3 5 1p
S3 N002 0 4 N002 C
S4 0 N002 N002 3 C
R3 3 2 1G noiseless
G1 0 N002 N003 0 {1/Rout}
R1 3 N002 {2*Rout} noiseless
R2 N002 4 {2*Rout} noiseless
C1 N002 0 {X*Cout/Avol}
S5 0 N003 N003 3 C
S6 N003 0 4 N003 C
R4 3 1 1G noiseless
R5 1 4 1G noiseless
R6 2 4 1G noiseless
.model C SW(Ron=100 Roff=1T Vt=0 Vh=-1 noiseless)
.param Rout=100Meg
.param Cout={Avol/GBW/2/pi/Rout}
.model Q SW(Ron=10 Roff=10Meg Vt=0 Vh=-.1 Vser={Rail}
ilimit={Ilimit} noiseless)
.param Avol=10Meg GBW=10Meg Slew=10Meg rail=0 Vos=0
ilimit=25m
.param en=0 enk=0 in=0 ink=0 phimargin=45
.param X
table(phimargin,29.4,3.5,32.1,2.9,33.8,2.6,35.8,2.3,38.1,2,40.9,1.7,43.2,1.5,45.9,1.3,49.2,1.1,53.2,0.9,58.2,0.7,64.7,0.5,73,0.3,86.1,0.05)
.ends 2pole


__________________________________________________
Do you Yahoo!?
Yahoo! Platinum - Watch CBS' NCAA March Madness, live on your desktop!
Re: New Feature Released & Opamp Modeling

Jonathan Kirwan
 

On Wed, 26 Mar 2003 00:49:55 -0800, you wrote:

Thanks. Just tested and it seems to work okay. Now what I'm
wondering about is what is displayed on the schematic. Should I
remove "visibility" for the Value attribute and add "visibility"
for the SpiceModel attribute on the underlying .ASY symbol?
I guess I'm asking this because the .ASY I currently use
automatically displays the Value attribute. But the new
drop-down for the SpiceModel only changes the SpiceModel
attribute (perhaps, as it should.) Since this isn't normally
displayed on the schematic, so far as I've seen anyway,
selecting a new model doesn't change what appears on the
schematic. So I have to manually change the Value attribute, as
well, in order to match (so it appears.)

For example, if I select 2N6028 in the drop-down for SpiceModel
*and* then manually change the Value attribute to match,
everything works well. If I then set the Value attribute to
"junk," leaving the SpiceModel to 2N6028, I get "Error: Unknown
subckt called in: xu1 n001 n002 n003 2N6028 junk" If I then try
and change the Value attribute to 2N6027 (which is also present
in the .LIB file I have, but which is *not* a match for the
current SpiceModel, which is 2N6028), then I get the error, "Too
many parameters for subcircuit type "2n6027" (instance: xu1)"

Just to let you know.

Jon
Re: New Feature Released & Opamp Modeling

Jonathan Kirwan
 

On Tue, 25 Mar 2003 15:19:26 -0800 (PST), you wrote:

Jon,

In the above case, it would be nice if LT Spice
would put a "Select Subcircuit" button on the
dialog box which comes up when I right-click on
the symbol (if the .ASY symbol is an X type)
and provide me a list of .SUBCKT entries it
found in the specified library file. In that
case, the PUJT.LIB case, this means it would pop
up 2N6027 and 2N6028, for example, and offer
those as options.
Yes, this is something that's been needed for a
long time. So I implemented it today. To use
it make a symbol with prefix 'X'. Make ModelFile
point to a library contianing subcircuits. Give
the symbol a SpiceModel that coincides with the
name of a subcircuit in ModelFile. Those
conditions will cause the editor for the
SpiceModel to be replaced with a drop list of
subcircuits in the file pointed to by ModelFile.

I modified the symbols 1pole.asy and 2pole.asy
to put the subcircuit names as the SpiceModel
attribute instead of the value so that you can
see it work(Though there's only one subcircuit
in the list to choose from). It's possible
that old schematics drafted with yesterday's
version don't work, just delete and replace the
1pole and 2pole instances to fix.
Thanks. Just tested and it seems to work okay. Now what I'm
wondering about is what is displayed on the schematic. Should I
remove "visibility" for the Value attribute and add "visibility"
for the SpiceModel attribute on the underlying .ASY symbol?

Jon
Suggestions for waveform viewer

Schaich, Peter
 

Hi there,


LTSpice is really fun to work with. Assuming that Mike likes to get
feedback, I would like to make some suggestions for enhancements of the
waveform viewer, mainly for documentation purposes:

* If any parameter of the circuit is stepped with the .step command, it
should be possible in the waveform viewer to see what value the parameter
has in the respective curve. (see example stempodelparam.asc) Preferably
on a legend that can be switched on or off.

* the number of the cursor should always be displayed, not only on
mouseover.

* maybe it should be possible to add some draw elements for documentation

* add a second color profile for the use of the results (via clipboard
copy) in other documents with white background and different colors for
grid, cursors and axis (cursor color is currently not customizable). There
is no doubt that black background is good for working on the screen but
white background is good for documentation.

What are your thoughts?

Regards

Peter Schaich
Re: Adding 3rd party Mosfet

 

--- In LTspice@..., "David Pariseau"
<david.pariseau@s...> wrote:
Helmut,

What's your email address? The one posted
is truncated with ...
Hello Dave,
sorry, but YAHOO shorted my e-mail address so that you had no chance
to fully read it.

HelmutSennewald"at"t-online.de
Replace "at" with @.

You can use my Yahoo address too, if it still doesn't work.
HelmutSennewald@...

Best Regards,
Helmut
TRIAC model

[email protected]
 

Hello,

I'm new to this group and I don't have experience working with
Spice models.

Someone can please help me or point me to the right direction so I
can make a TRIAC model? If there's some ready-to-go model, please let me
know.

Thank you very much,

Brusque

--
-----------------------------------------------------------------
Edson Brusque C.I.Tronics Lighting Designers Ltda
Research and Development Blumenau - SC - Brazil
Say NO to HTML mail www.citronics.com.br
-----------------------------------------------------------------
Re: Adding 3rd party Mosfet

David Pariseau
 

Helmut,

What's your email address? The one posted
is truncated with ...

Dave.
Re: Using Field Sync about the Globe

 

There's been some reorganization of
the website that I use of SwCADIII/LTspice
publication. Could you folks let me
know if the menu item Tools=>Sync Release
works for you. It should work from
anywhere in the world and give you
version 2.01s right now.

Probably better to e-mail me at
pmte@..., instead of posting
to the users' group.

--Mike

__________________________________________________
Do you Yahoo!?
Yahoo! Platinum - Watch CBS' NCAA March Madness, live on your desktop!
Re: Adding 3rd party Mosfet

 

Helmut,

Hello Mike or whoever exactly knows about,
...if a model uses the node number 0, is
it then referenced to the common ground
0 of the top schematic or is this a
floating node like any other node inside
the subcircuit?
Yes you are correct, node 0 is global.
Even if used in a subcircuit, it is global
ground. You can't name the pin of a
hierarchical symbol "0" and have that
refer to the node "0" inside that page of
circuitry.

Note that you can specify other nodes to
be globals with the .global dot command.

--Mike

__________________________________________________
Do you Yahoo!?
Yahoo! Platinum - Watch CBS' NCAA March Madness, live on your desktop!
Re: Setting or Freezing Plot Scales

 

Steve,

First let me congratulate the author(s) and those
that support this software. It is really useful
and easy to use.
Thanks!

My daughter, who is an engineering sophomore,
has even started to use LTSpice for some labs.
Cool. Just the same, I don't think we should risk
having a slogan like, "So easy to use even girls can
use it."

I am looking for a way to either pass plot scales
from a dot statement (.PLOT or .VIEW kind of thing)
or at least to freeze the plot scales from run to
run. It would be helpful when trying to visually
compare the the results between runs if the the
plot did not automatically rescale. It would also
be nice to be able to have an alias type statement
to save reentering things like V(out)/V(in) or
V(N003, N006)/I(R7).
Yes, I we will be making it possible to have named
plot setups and turn off autoscaling. I was planing
on starting that today, but this programmable library
became important because it changes some standards
used.

--Mike

__________________________________________________
Do you Yahoo!?
Yahoo! Platinum - Watch CBS' NCAA March Madness, live on your desktop!
Re: New Feature Released & Opamp Modeling

 

Jon,

In the above case, it would be nice if LT Spice
would put a "Select Subcircuit" button on the
dialog box which comes up when I right-click on
the symbol (if the .ASY symbol is an X type)
and provide me a list of .SUBCKT entries it
found in the specified library file. In that
case, the PUJT.LIB case, this means it would pop
up 2N6027 and 2N6028, for example, and offer
those as options.
Yes, this is something that's been needed for a
long time. So I implemented it today. To use
it make a symbol with prefix 'X'. Make ModelFile
point to a library contianing subcircuits. Give
the symbol a SpiceModel that coincides with the
name of a subcircuit in ModelFile. Those
conditions will cause the editor for the
SpiceModel to be replaced with a drop list of
subcircuits in the file pointed to by ModelFile.

I modified the symbols 1pole.asy and 2pole.asy
to put the subcircuit names as the SpiceModel
attribute instead of the value so that you can
see it work(Though there's only one subcircuit
in the list to choose from). It's possible
that old schematics drafted with yesterday's
version don't work, just delete and replace the
1pole and 2pole instances to fix.

--Mike

__________________________________________________
Do you Yahoo!?
Yahoo! Platinum - Watch CBS' NCAA March Madness, live on your desktop!
Re: Adding 3rd party Mosfet

 

--- In LTspice@..., "David Pariseau"
<david.pariseau@s...> wrote:
Hello Dave,
this model from Fairchild has 4 pins. Please add a 4th pin to
your
symbol. You can see that requirement in the model file. I tried
this with success.

*20=DRAIN 10=GATE 30=SOURCE 50=VTEMP
.SUBCKT FDN304p 20 10 30 50
That's weird, the part is in an SOT-3 package w/ only 3 pins,
but it seems that the 4th input is temperature???

It has been also necessary to add a resistor to this additionally
node in the schematic. I connected a 1k resistor to ground in my
test circuit. This works at least for circuits where the drain is
connected to >=0V.
I added this and commented out the Diode line and there are no
errors
now in simulation, but the simulation is glacially slow and I'm not
sure correct.
Hello David,
you can send me your circuit file(s) for testing.
Please use the following e-mail address if you are interested.
HelmutSennewald@...

Best Regards
Helmut
Re: Adding 3rd party Mosfet

David Pariseau
 

Hello Dave,
this model from Fairchild has 4 pins. Please add a 4th pin to your
symbol. You can see that requirement in the model file. I tried
this with success.

*20=DRAIN 10=GATE 30=SOURCE 50=VTEMP
.SUBCKT FDN304p 20 10 30 50
That's weird, the part is in an SOT-3 package w/ only 3 pins,
but it seems that the 4th input is temperature???

It has been also necessary to add a resistor to this additionally
node in the schematic. I connected a 1k resistor to ground in my
test circuit. This works at least for circuits where the drain is
connected to >=0V.
I added this and commented out the Diode line and there are no errors
now in simulation, but the simulation is glacially slow and I'm not
sure correct.

Thanks for the input, Helmut,
Dave Pariseau.
Re: Adding 3rd party Mosfet

 

--- In LTspice@..., "David Pariseau"
<david.pariseau@s...> wrote:
I've read through past messages, the SwCAD help
and such and attempted to add a 3rd party model
for the FDN304P. It seems to find the model fine
now, but I get the error "Too few parameters for
subcircuit type "fdn304p"".

I basically dropped the model file into the &#92;sub
directory, copied the pmos symbol file and changed
it to specify the FDN304p model.

Hello Dave,
this model from Fairchild has 4 pins. Please add a 4th pin to your
symbol. You can see that requirement in the model file. I tried this
with success.

*20=DRAIN 10=GATE 30=SOURCE 50=VTEMP
.SUBCKT FDN304p 20 10 30 50

It has been also necessary to add a resistor to this additionally
node in the schematic. I connected a 1k resistor to ground in my test
circuit. This works at least for circuits where the drain is
connected to >=0V.

Fairchilds fault?
The model has a badly designed breakdown section.
It shorts the drain if it is below zero volt relative to ground. So
it is unusable in this case. If you have a need for this then you can
comment the line with the diode D.

*D DB1 20 DBLK

Now it will run with a voltage below 0V too, but the breakdown is no
more modelled.

Original section:
*DIODE THERMO BREAKDOWN SECTION
EBL VB1 VB2 101 0 0.8
VBLK VB2 0 20
D DB1 20 DBLK
.MODEL DBLK D(IS=1E-14 CJO=.1p RS=.1)
EDB 0 DB1 VB1 0 1



Hello Mike or whoever exactly knows about,
if a model uses the node number 0, is it then referenced to the
common ground 0 of the top schematic or is this a floating node like
any other node inside the subcircuit?

Best Regards
Helmut
Re: New Feature Released & Opamp Modeling

cadencespectre
 

--- In LTspice@..., "Reinier Gerritsen" <r.gerritsen@c...>
wrote:

SNIP

- a way to store multiple analysis commands. If I use .tran and .ac
commands, only the parameters of the last one is saved, the other
gets lost
on exit of the program.

Thanks for you great software and support.

Reinier Gerritsen
The Netherlands
Hoi Reinier,

It is possible to save multiple analysis commands. First place a
simulation command on the sheet. When you add a second simulation
command with Simulate -> Edit Simulation Command (or right mouse
button -> Edit Simulation Command), and place the command on the
sheet, you'll see the "." in the first comman will change to ";".
E.g. you'll get:

.tran 10n
;ac dec 51 100 10G
;dc temp -40 125 2

If you save this schematic, and reopen it, you can choose using
Simulate -> Edit Simulation Command (or right mouse button -> Edit
Simulation Command).
It only works for different analysis types. I.e. you can't choose
between e.g. multiple .tran commands (however you can uncomment them).
Of course you can place these lines on the schematic manually.

Regards,

Ronnie (Also from the Netherlands :-) )
Adding 3rd party Mosfet

David Pariseau
 

I've read through past messages, the SwCAD help
and such and attempted to add a 3rd party model
for the FDN304P. It seems to find the model fine
now, but I get the error "Too few parameters for
subcircuit type "fdn304p"".

I basically dropped the model file into the &#92;sub
directory, copied the pmos symbol file and changed
it to specify the FDN304p model.

Any thoughts?
Dave Pariseau.

Here are the files:

FDN304p.asy
-------------
Version 4
SymbolType CELL
LINE Normal 48 48 48 96
LINE Normal 16 80 48 80
LINE Normal 16 48 24 48
LINE Normal 48 48 24 44
LINE Normal 48 48 24 52
LINE Normal 24 44 24 52
LINE Normal 16 8 16 24
LINE Normal 16 40 16 56
LINE Normal 16 72 16 88
LINE Normal 0 80 8 80
LINE Normal 8 16 8 80
LINE Normal 48 16 16 16
LINE Normal 48 0 48 16
WINDOW 0 56 32 Left 0
WINDOW 3 56 72 Left 0
SYMATTR Value FDN304P
SYMATTR Prefix X
SYMATTR SpiceModel FDN304P.mod
SYMATTR Value2 FDN304P
SYMATTR Description P-Channel MOSFET transistor
PIN 48 0 NONE 0
PINATTR PinName D
PINATTR SpiceOrder 1
PIN 0 80 NONE 0
PINATTR PinName G
PINATTR SpiceOrder 2
PIN 48 96 NONE 0
PINATTR PinName S
PINATTR SpiceOrder 3

FDN304p.mod
---------------
*FDN304P at Temp. Electrical Model (T2)
*-------------------------------------
.SUBCKT FDN304p 20 10 30 50
*20=DRAIN 10=GATE 30=SOURCE 50=VTEMP
Rg 10 11x 1
Rdu 12x 1 1u
M1 2 1 4x 4x DMOS L=1u W=1u
.MODEL DMOS PMOS(VTO=-0.87 KP=2.5E+1
+THETA=0.25 VMAX=8.5E5 LEVEL=3)
Cgs 1 5x 1300p
Rd 20 4 7E-3
Dds 4 5x DDS
.MODEL DDS D(M=4.26E-1 VJ=3.39E-1 CJO=562p)
Dbody 20 5x DBODY
.MODEL DBODY D(IS=3.81E-10 N=1.145283 RS=0.00084 TT=14.5n)
Ra 4 2 7E-3
Rs 5x 5 0.5m
Ls 5 30 0.5n
M2 1 8 6 6 INTER
E2 8 6 4 1 2
.MODEL INTER PMOS(VTO=0 KP=10 LEVEL=1)
Cgdmax 7 4 1050p
Rcgd 7 4 10meg
Dgd 4 6 DGD
Rdgd 4 6 10meg
.MODEL DGD D(M=3.2E-1 VJ=4.23E-3 CJO=1050p)
M3 7 9 1 1 INTER
E3 9 1 4 1 -2
*ZX SECTION
EOUT 4x 6x poly(2) (1x,0) (3x,0) 0 0 0 0 1
FCOPY 0 3x VSENSE 1
RIN 1x 0 1G
VSENSE 6x 5x 0
RREF 3x 0 10m
*TEMP SECTION
ED 101 0 VALUE {V(50,100)}
VAMB 100 0 25
EKP 1x 0 101 0 .012
*VTO SECTION
EVTO 102 0 101 0 .0007
EVT 11x 12x 102 0 1
*DIODE THERMO BREAKDOWN SECTION
EBL VB1 VB2 101 0 0.8
VBLK VB2 0 20
D DB1 20 DBLK
.MODEL DBLK D(IS=1E-14 CJO=.1p RS=.1)
EDB 0 DB1 VB1 0 1
.ENDS FDN304p
*FDN304P (Rev.A) 12/4/00 **ST
157581 - 157600 of 157803