I can't seem to get this model for a TLC555 (555 timer
IC) to work correctly, the output is pegged at 12v.

Any thoughts?
Dave.


***
* TLC555 TIMER MACROMODEL
**
4/1/92****
DBB
* REV N/A
***

***
* COMMON
* | TRIGGER
* | | OUTPUT
* | | | RESET
* | | | | CONTROL
* | | | | | THRESHOLD
* | | | | | | DISCHARGE
* | | | | | | | VDD
* | | | | | | | |
.SUBCKT TLC555 1 2 3 4 5 6 7 8
EREF 15 1 (8,1) .5
GSOURCE 8 3 (8,26) 12.5E-3
GSINK 3 1 (26,1) 67E-3
VD1 8 27 DC .8
VD2 28 1 DC .85
VREF 30 1 DC 1.2
C1 29 1 700E-15
RREF2 30 1 100E3
RREF 15 1 100E3
ROUT 3 1 100K
R1 6 1 500E9
R2 2 1 500E9
R3 8 5 75E3
R4 5 9 75E3
R5 9 1 75E3
R6 10 11 1E3
R7 13 14 1E3
R8 8 12 150E3
R9 4 8 500E9
R10 20 19 1E3
R11 16 17 1E3
R12 8 18 150E3
R13 8 21 150E3
R14 22 23 1E3
R15 8 26 150E3
R16 24 25 1E3
R19 7 1 500E9
R20 29 26 1E6
D1 1 11 DMOD
D2 12 11 DMOD
D3 12 14 DMOD
D4 1 14 DMOD
D5 18 17 DMOD
D6 1 17 DMOD
D7 18 19 DMOD
D8 1 19 DMOD
D9 21 14 DMOD
D10 21 25 DMOD
D11 1 23 DMOD
D12 18 23 DMOD
D13 26 25 DMOD
D14 1 25 DMOD1
D15 3 27 DMOD
D16 28 3 DMOD
E1 10 1 (6,5) 1000
E2 13 1 (2,9) 1000
E3 16 1 (15,12) 1000
E4 22 1 (15,21) 1000
E5 24 1 (15,18) 1000
E7 20 1 (4,30) 1000
M1 7 29 1 1 MOSMOD
.MODEL MOSMOD NMOS (LEVEL=1 KP=1 VTO=1 RD=5)
.MODEL DMOD D (RS=1E-6)
.MODEL DMOD1 D (RS=1E-6 IS=1E-9)
.ENDS

Symbol
------------------------
Version 4
SymbolType CELL
RECTANGLE Normal 192 46 -159 -253
WINDOW 0 17 -144 Center 0
WINDOW 3 17 -103 Center 0
SYMATTR Value X_555
SYMATTR Prefix X
PIN 16 48 BOTTOM 10
PINATTR PinName GND
PINATTR SpiceOrder 1
PIN -160 -64 LEFT 10
PINATTR PinName TRIG
PINATTR SpiceOrder 2
PIN 192 -144 RIGHT 10
PINATTR PinName OUT
PINATTR SpiceOrder 3
PIN 80 -256 TOP 8
PINATTR PinName RESET
PINATTR SpiceOrder 4
PIN 192 -16 RIGHT 10
PINATTR PinName CONT
PINATTR SpiceOrder 5
PIN -160 -96 LEFT 10
PINATTR PinName THRESH
PINATTR SpiceOrder 6
PIN -160 -208 LEFT 10
PINATTR PinName DISCH
PINATTR SpiceOrder 7
PIN -32 -256 TOP 8
PINATTR PinName VDD
PINATTR SpiceOrder 8

Schematic
------------------------
Version 4
SHEET 1 880 680
WIRE -496 32 -496 48
WIRE -496 -48 -496 -64
WIRE 32 320 32 288
WIRE -144 176 -304 176
WIRE -144 144 -256 144
WIRE -304 144 -304 128
WIRE -304 176 -304 144
WIRE -304 32 -256 32
WIRE -304 48 -304 32
WIRE -304 -48 -304 -64
WIRE -304 -64 -16 -64
WIRE -16 -64 -16 -16
WIRE 96 -16 96 -64
WIRE 96 -64 -16 -64
WIRE -304 -64 -496 -64
WIRE 256 240 256 224
WIRE 256 224 208 224
WIRE 208 96 304 96
WIRE -256 64 -256 32
WIRE -256 32 -144 32
WIRE -256 128 -256 144
WIRE -256 144 -304 144
FLAG 32 320 0
FLAG -496 48 0
FLAG 256 304 0
FLAG -304 240 0
FLAG 304 96 VOUT
SYMBOL C:\Program\ Files\LTC\SwCADIII\lib\sym\voltage -496 -64 R0
WINDOW 123 0 0 Left 0
WINDOW 39 0 0 Left 0
WINDOW 0 37 42 Left 0
WINDOW 3 36 64 Left 0
SYMATTR InstName V1
SYMATTR Value 12V
SYMBOL C:\Program\ Files\LTC\SwCADIII\lib\sym\res -320 -64 R0
WINDOW 0 -50 45 Left 0
WINDOW 3 -55 74 Left 0
SYMATTR InstName R1
SYMATTR Value 1.8K
SYMBOL C:\PROGRAM\ FILES\LTC\SWCADIII\lib\sym\res -320 32 R0
WINDOW 0 -42 37 Left 0
WINDOW 3 -48 69 Left 0
SYMATTR InstName R2
SYMATTR Value 1.8K
SYMBOL C:\PROGRAM\ FILES\LTC\SWCADIII\lib\sym\Misc\x_555 16 240 R0
WINDOW 0 4 -144 Center 0
WINDOW 3 2 -99 Center 0
SYMATTR InstName U1
SYMATTR Value TLC555
SYMATTR SpiceModel TLC555
SYMBOL C:\PROGRAM\ FILES\LTC\SWCADIII\lib\sym\cap 240 240 R0
WINDOW 0 43 23 Left 0
WINDOW 3 42 51 Left 0
SYMATTR InstName C1
SYMATTR Value 0.01?f
SYMBOL C:\PROGRAM\ FILES\LTC\SWCADIII\lib\sym\cap -320 176 R0
WINDOW 0 -38 32 Left 0
WINDOW 3 -57 57 Left 0
SYMATTR InstName C2
SYMATTR Value 0.1?f
SYMBOL C:\PROGRAM\ FILES\LTC\SWCADIII\lib\sym\diode -272 64 R0
WINDOW 0 41 24 Left 0
WINDOW 3 39 50 Left 0
SYMATTR InstName D1
SYMATTR Value 1N4148
TEXT -162 346 Left 0 !.tran 500ms
TEXT -288 384 Left 0 !.include "c:\program
files\ltc\swcadiii\lib\sub\ti.lib"

Helmut,

Anyone got a way of doing a monte carlo run (AC or AC sweep)
using the resistor and capacitance tolerances?

Those tolerances are just for the bill of material, like
the partnumber and mfg.

About as close as you can get to doing Monte Carlo in LTspice
is with parameterized curly brace expressions using the rand()
function. Attached is an example.

Hello Mike,
I like your example. Could you put it into the Example\Educational
folder of LTSPICE?

Only one correction of this schematic.

OK, will do after making the correction. I might also make it
a narrower filter so the analysis is a bit more interesting.

--Mike

__________________________________________________
Do you Yahoo!?
Yahoo! Tax Center - File online, calculators, forms, and more

--- In LTspice@..., Panama Mike <panamatex@y...> wrote:

Brian,

Anyone got a way of doing a monte carlo run (AC or AC sweep)
using the resistor and capacitance tolerances?

Those tolerances are just for the bill of material, like
the partnumber and mfg.

About as close as you can get to doing Monte Carlo in LTspice
is with parameterized curly brace expressions using the rand()
function. Attached is an example.

Hello Mike,
I like your example. Could you put it into the Example&#92;Educational
folder of LTSPICE?

Only one correction of this schematic.

> SYMATTR Value {1n*(1+a*(rand(x+600)-.5))}
> !.param a=.2 ; 20% component tolerance

This line should have the comment 10% and not 20% for the used
formula {1n*(1+a*(rand(x+600)-.5))}) .

The reason is the used function (rand(x+400)-.5)) gives only
values from -0.5 to +0.5 .

Normally we always have +/-tolerance of passive components. If a
component is specified with 10% tolerance, then it has a tolerance of
+/-10%.


We could also adjust the formula by a factor of 2 instead.
> SYMATTR Value {1n*(1+2*a*(rand(x+600)-.5))}
Now we will get +/-20% tolerance for a = 0.2 .

Best Rgeards
Helmut

Brian,

Anyone got a way of doing a monte carlo run (AC or AC sweep)
using the resistor and capacitance tolerances?

Those tolerances are just for the bill of material, like
the partnumber and mfg.

About as close as you can get to doing Monte Carlo in LTspice
is with parameterized curly brace expressions using the rand()
function. Attached is an example.

--Mike

--- MonteCarlo.asc ---
Version 4
SHEET 1 1268 692
WIRE -512 368 -512 336
WIRE -512 256 -512 240
WIRE -512 240 -400 240
WIRE -112 240 -48 240
WIRE 880 240 880 272
WIRE 880 336 880 368
WIRE 800 240 800 272
WIRE 800 352 800 368
WIRE 800 240 880 240
WIRE -48 240 -48 272
WIRE -48 336 -48 368
WIRE -112 240 -112 272
WIRE -112 352 -112 368
WIRE -48 240 160 240
WIRE -320 240 -112 240
WIRE 1200 368 1200 352
WIRE 1200 272 1200 240
WIRE 1200 240 880 240
WIRE 240 240 528 240
WIRE 592 240 800 240
FLAG 880 368 0
FLAG -512 368 0
FLAG 800 368 0
FLAG -48 368 0
FLAG -112 368 0
FLAG 1200 368 0
SYMBOL cap 864 272 R0
SYMATTR InstName C1
SYMATTR Value {1n*(1+a*(rand(x+600)-.5))}
SYMBOL voltage -512 240 R0
SYMATTR InstName V1
SYMATTR Value AC 1
SYMBOL ind 816 256 M0
SYMATTR InstName L1
SYMATTR Value {10u*(1+a*(rand(x+500)-.5))}
SYMBOL cap -64 272 R0
SYMATTR InstName C2
SYMATTR Value {1n*(1+a*(rand(x+100)-.5))}
SYMBOL ind -96 256 M0
SYMATTR InstName L2
SYMATTR Value {10u*(1+a*(rand(x)-.5))}
SYMBOL res -304 224 R90
WINDOW 0 0 56 VBottom 0
WINDOW 3 32 56 VTop 0
SYMATTR InstName R1
SYMATTR Value 100
SYMBOL res 1184 368 M180
WINDOW 0 36 76 Left 0
WINDOW 3 36 40 Left 0
SYMATTR InstName R2
SYMATTR Value 100
SYMBOL ind 256 256 M270
WINDOW 0 32 56 VTop 0
WINDOW 3 5 56 VBottom 0
SYMATTR InstName L3
SYMATTR Value {20u*(1+a*(rand(x+300)-.5))}
SYMBOL cap 592 224 R90
WINDOW 0 0 32 VBottom 0
WINDOW 3 32 32 VTop 0
SYMATTR InstName C3
SYMATTR Value {500p*(1+a*(rand(x+400)-.5))}
TEXT -264 504 Left 0 !.ac oct 100 300K 10Meg
TEXT 160 488 Left 0 !.step param X 0 20 1
TEXT 160 464 Left 0 !.param a=.2 ; 20% component tolerance


__________________________________________________
Do you Yahoo!?
Yahoo! Tax Center - File online, calculators, forms, and more

Anyone got a way of doing a monte carlo run (AC or AC sweep) using the
resistor and capacitance tolerances ?


Brian

--
Brian Howie | Tel: 0131 343 5590
BAE SYSTEMS | Fax: 0131 343 5050
Sensor Systems Division | Email brian.howie@...
Silverknowes | bhowie@...
Edinburgh EH4 4AD | Web site www.baesystems.com


***
This email and any attachments are confidential to the intended
recipient and may also be privileged. If you are not the intended
recipient please delete it from your system and notify the sender.
You should not copy it or use it for any purpose nor disclose or
distribute its contents to any other person.
***

Russell,

Is the recently added 'GMIN across Current Sources'
hack needed when using the Lin Tech Op Amp models in
LTC.lib?

I ask this because in times gone by the Lin Tech
SPICE Model Library came with a copy of the demo
version of PSPICE on the disk and presumably the
models were written (and tested?) with that
simulator in mind.

I wouldn't take the opamp models in LTC.lib so seriously
as to worry about whether 'GMIN across Current Sources'
was checked or not. The model for wish that got introduced
for was pretty silly. It would only work if gmin was
equal to the default of 1e-12. The model would break
if you needed to adjust it for some special considerations.
Pretty lame overall since that opamp was made for
electrometer applications.

--Mike


__________________________________________________
Do you Yahoo!?
Yahoo! Tax Center - File online, calculators, forms, and more

Greetings All,

I have a question for Mike E...

Mike,

Is the recently added 'GMIN across Current Sources' hack needed when
using the Lin Tech Op Amp models in LTC.lib?

I ask this because in times gone by the Lin Tech SPICE Model Library
came with a copy of the demo version of PSPICE on the disk and
presumably the models were written (and tested?) with that simulator
in mind.

Thanks

Russell

开云体育

Reinier,

> I use the .step command to do multiple .AC runs. One of
> the inductances in my circuit is swept.? How do I know
> which trace belongs to which step value?? Do I have to
> count the traces? I want to use some 50 traces at the
> same time, just a small frequency span. Could the
> trace number be displayed or better, the corresponding
> inductance be displayed in the cursor window?

If you want to use many inductance values, at one frequency
of interest then you can have the frequency component
plotted as a function of inductance this automatically
happens when you do a .step for a .ac with only one data
point.? The following deck will illustrate:

*
L1 N001 N002 {L}
R1 N002 0 1K
V1 N001 0 ac 1
.ac list 10Meg
.step param L 10u 1000u 10u
.end

However, if you do a .step and there is whole data set
at each .step point, then there's no easy way to identify
which trace goes with which step.? You basically have to
count.? The attached cursor helps some here in that the
up/down arrow keys will make the attached cursor jump
from one .step to the next.

--Mike?

?

Reinier,

I use the .step command to do multiple .AC runs. One of
the inductances in my circuit is swept. How do I know
which trace belongs to which step value? Do I have to
count the traces? I want to use some 50 traces at the
same time, just a small frequency span. Could the
trace number be displayed or better, the corresponding
inductance be displayed in the cursor window?

If you want to use many inductance values, at one frequency
of interest then you can have the frequency component
plotted as a function of inductance this automatically
happens when you do a .step for a .ac with only one data
point. The following deck will illustrate:

*
L1 N001 N002 {L}
R1 N002 0 1K
V1 N001 0 ac 1
.ac list 10Meg
.step param L 10u 1000u 10u
.end

However, if you do a .step and there is whole data set
at each .step point, then there's no easy way to identify
which trace goes with which step. You basically have to
count. The attached cursor helps some here in that the
up/down arrow keys will make the attached cursor jump
from one .step to the next.

--Mike

__________________________________________________
Do you Yahoo!?
Yahoo! Tax Center - File online, calculators, forms, and more

Thanks for all the leads on this one, I'll see what I can come up with.
Thanx,
-Jon

--------------------------------------------------------------------------
Jonathan W. T. Graham grambo@...

Design Engineer with Oztek Corp.
WPI/NASA GSFC Global Precipitation Mission 603.622.6402x205
Intel IXP1200 Applications Team Alumnus fax 425.920.7258

Hi,

I use the .step command to do multiple .AC runs. One of the inductances in
my circuit is swept. How do I know which trace belongs to which step value?
Do I have to count the traces? I want to use some 50 traces at the same
time, just a small frequency span. Could the trace number be displayed or
better, the corresponding inductance be displayed in the cursor window?

Reinier

Hi,

I use a free utility from IntuSoft called IBIS2SPICE.

It reads in IBIS models (up to version 2.1) and generates an equivalent behavioural spice model. It's originally intended to generate a model compatible with Intusoft's spice, but can be configureed to generate models for other spices based on a template file. There's a templeate file available on the net somewhere to configure it for PSpice models.

I can't really vouch for the accuracy of the models it generates, and it's limited to IBIS version 2.1.

Generally it would be a great feature to have in LTSpice, but I guess it's not a priority for LT's chip designers, IBIS tends to be used primarily by board designers for board level Signal Integity analysis.

Robert


--
Robert Lindsell, Principal Hardware Engineer
Canon Information Systems Research Australia
PO Box 313 NORTH RYDE NSW 2113
mailto:robert.lindsell@...
Fax: +61-2-9805-2929 Phone: +61-2-9805-2876


Panama Mike wrote:

--- In LTspice@..., "Jonathan Graham" <jgraham@o...>
wrote:

Is there any support for IBIS models in LTSpice? Assuming that

there isn't,

are there any suggestions for what to do if a manufacturer only has

an IBIS

model for a part that I'd like to model?
Specifically, I'm looking to model the drive capabilities of the

74lvth245

and 74lvc1g125 from TI to see how cleanly they can drive a spi bus

with some

50 or 60 devices on it.

Hello Jonathan,
I have seen SPICE models of similar ICs on the Philips web site,
but I am not shure how compatible they are.


Best Regards
Helmut

Jon,

Is there any support for IBIS models in LTSpice? Assuming
that there isn't, are there any suggestions for what to do
if a manufacturer only has an IBIS model for a part that
I'd like to model? Specifically, I'm looking to model the
drive capabilities of the 74lvth245 and 74lvc1g125 from TI
to see how cleanly they can drive a spi bus with some
50 or 60 devices on it.

No, IBIS isn't in LTspice. I think IBIS was an Intel
invention that allowed them to give behavioral descriptions
of their I/O pins without giving out implementation details.

Anyway, I think IBIS amounts largely to an IV curve.
The DC curve you can put in an IV lookup table. To do
the dynamic behavior, you're better off with some kind
of transistor level model of the device. Attached is
an example of using a lookup table in a current source.
I don't know if it's otherwise documented anywhere.

Version 4
SHEET 1 880 680
WIRE -32 320 -32 288
WIRE -32 208 -32 176
WIRE -32 176 -160 176
WIRE -160 176 -160 208
WIRE -160 288 -160 320
FLAG -160 320 0
FLAG -32 320 0
SYMBOL current -32 208 R0
SYMATTR InstName I1
SYMATTR Value tbl(-5 -1 -2 -.5 0 0 1 1 5 2)
SYMBOL voltage -160 192 R0
SYMATTR InstName V1
SYMATTR Value 0
TEXT -152 368 Left 0 !.dc V1 -5 5 1m

--Mike

__________________________________________________
Do you Yahoo!?
Yahoo! Tax Center - File online, calculators, forms, and more

Bill,

What sort of things would one do to minimize
the time required to process a simulation?

I think it might be hard to generalize without
seeing the circuit that's causing you trouble.
Usually its a matter of finding the part of the
circuit that's causing difficulty and find a
different way to model it. Other than that,
here are some things to try.

1. Simplify the circuit, reduce node count,
remove floating voltage sources.
2. Setting trtol to 7(the default in most SPICE's
unlike LTspice's 1)
3. Use initial conditions so that the circuit doesn't
have to run as long to get to that aspect of the
circuit's behavior that your interested in.
4. Replace behavioral(A-source) models with real
devices if possible.

--Mike

__________________________________________________
Do you Yahoo!?
Yahoo! Tax Center - File online, calculators, forms, and more

Is there any support for IBIS models in LTSpice? Assuming that there isn't,
are there any suggestions for what to do if a manufacturer only has an IBIS
model for a part that I'd like to model?
Specifically, I'm looking to model the drive capabilities of the 74lvth245
and 74lvc1g125 from TI to see how cleanly they can drive a spi bus with some
50 or 60 devices on it.
Thanx,
-Jon

--------------------------------------------------------------------------
Jonathan W. T. Graham grambo@...

Design Engineer with Oztek Corp.
WPI/NASA GSFC Global Precipitation Mission 603.622.6402x205
Intel IXP1200 Applications Team Alumnus fax 425.920.7258

What sort of things would one do to minimize the time
required to process a simulation?

Bill



__________________________________________________
Do you Yahoo!?
Yahoo! Tax Center - File online, calculators, forms, and more

Steve,

Mike, is there a way to tell which plot window will be
updated when the simulation is re-run? ie, Which is
considered the active plot window? Also, is there a
way to get all plot windows to update on re-running the
simulation in case you use this feature to be able to
clearly see multiple traces?

Multiple plot windows were a precursor to the multiple
pane plots that are now supported. The active window
is the one most recently opened. Whether adding plot
a trace to an old window will be the old data or
new simulation data will depend on some non-obvious
things. Real data(not .ac) are disk based data. Whether
you see old data or new data bepends on what the view
has cached from the disk and there is no certain way
of knowing becuase it has it's own stategy how to
cache data depending on how much RAM you have. But
for .ac analysis, the data is not disk based so you
can keep old windows with old data in them.

Hope this helps,

--Mike

__________________________________________________
Do you Yahoo!?
Yahoo! Tax Center - File online, calculators, forms, and more

I just discovered (maybe everyone else already knew) that if you
choose View / Simulation Data after a plot is displayed, you get a
second independant plot window. If you rerun a simulation, only the
last plot window you opened will update. You can update other plot
windows by deleting and then adding the trace. This is handy for
comparing the results of changes to the circuit.

A word of caution, it looks like only the trace being displayed is
of the old run. If you add a trace to this plot window, it will
come from the new data (RAW file). It does not appear that you can
get the same node name to display twice (old and new) on one
Window. This can get rather confusing as there is no clear
indication of what is old data and what is new data so use this
feature (?) carefully. Similar results could be achieved with
access to all nodes and loops of the old run by having multiple
instances of the simulation open, each with a different name.

Mike, is there a way to tell which plot window will be updated when
the simulation is re-run? ie, Which is considered the active plot
window? Also, is there a way to get all plot windows to update on
re-running the simulation in case you use this feature to be able to
clearly see multiple traces?

Hello,
I have uploaded an enhanced version of the raw file utility program
ltsputil.exe. It allows you to convert, merge, equalize and export
your LTSPICE simulation raw files to other programs. Now it can
process swept simulations too. Especially the export function has
been greatly enhanced. The program runs still in the DOS box.
Take a look to the help file in the "Files" download area for the new
features.

Version 2.0 is very compatible for most options, but the export
option -x needs one paramter more now.

I have also uploaded the last freeware version(1.3) of the graphic
program DPLOT95.zip. This is the only version running under W2000.
All older version will fail. Newer versions are no more freeware but
at a reasonable price(www.dplot.com). I have no connection to this
company.

Have fun with these programs.

Best Regards
Helmut