
This an old posting I found.  It is the basis of how I created the LM741 device.  See below

====================
====================
====================


 "Chaos Master" <raw_chaos@brasnet.org > wrote in message

news:MPG.19a4f845ec428002989736@news.cis.dfn.de...

> Joe mumbled:
> > I have been using LTSPICE for a few weeks now and it is a great help in
> > figuring out how a circuit will work before breadboarding it. I am a
> > hobbyist and I work mostly with discretes and 555 timers along with some
> > cmos counters. Pretty simple stuff.
> > I have been reading the help file and also looked at some of the .lib
files
> > trying to figure out how to create some of my own components. I would
like
> > to add a cmos 556 to the library and possibly a few opamps that I am
> > familiar with (eg, 741) , but don't know where to start.
> > Is anyone familiar enough with creating custom components in this
simulator
> > to be able to steer me in the right direction??
>
> You'll need the models, and probably will need to create symbols.
> Search on Google for 'spice models'.
>
> --
> "* <- Tribble .SUBCKT * <- SPICE tribble."
> E-mail address is fake. Please reply to the group!

Thanks for the advice, already been there, done that. Problem is, there's so
many different models and whats the difference between HSPICE, and PSPICE ?.
I guess I need to know which model type is compatible with LTSPICE

. I thought I would be able to create one from one of the existing models
already in LTSPICE. They have a schematic for the 741 opamp in the
'educational' folder and it has pinouts. I dont find a .sub file for it tho.
I was able to read the .sub files for most of the models they have in there,
but I don't know what language it is written in. Are all spice models
compatible with all the simulators??

I downloaded a model for the LM741 opamp from the national semiconductor
site, but now don't know what to do with it. It looks a lot different then
the models I have been able to read in the LTSPICE folder.

I also found what looks like it may be a model of the 556 timer, but I have
to dl 'circuitmaker' student version. That simulator seems to have the most
models and is a freebie. I am just wondering if anyone uses it here, and if
maybe that would be the best route to go? I like using LTSPICE, but I guess
I need more information then what they give us in the help files unless
someone here is knowledgeable about creating new models for it. Or modifying
the existing models with the right parameters to get where I need to be.

Thank you again for the reply,

Joe







14 Aug 2003 21:53:53
Helmut Sennewald
Re: Need help with LTSPICE library

"Joe" <nuisancewildlife@nospamearthlink.net > schrieb im Newsbeitrag
news:uAA_a.13045$BC2.3380@newsread2.news.atl.earthlink.net...
> I have been using LTSPICE for a few weeks now and it is a great help in
> figuring out how a circuit will work before breadboarding it. I am a
> hobbyist and I work mostly with discretes and 555 timers along with some
> cmos counters. Pretty simple stuff.
> I have been reading the help file and also looked at some of the .lib
files
> trying to figure out how to create some of my own components. I would like
> to add a cmos 556 to the library and possibly a few opamps that I am
> familiar with (eg, 741) , but don't know where to start.
> Is anyone familiar enough with creating custom components in this
simulator
> to be able to steer me in the right direction??
>

Hello Joe,
here is the fastest route to your models in LTSPICE.

First you should create two new folders for your own models.
For the SPICE model:
C:ProgrammeLtcSwCADIIIlibsubPrivate
For the symbols:
C:ProgrammeLtcSwCADIIIlibsymPrivate

The let's start here at National.
http://www.national.com/appinfo/amps/0,2175,815,00.html
Download the LM741.mod into the new folder "Private" of LTSPICE
C:ProgrammeLtcSwCADIIIlibsubPrivate
We have then C:ProgrammeLtcSwCADIIIlibsubPrivatelm741.mod .
This is the Spice model file. Don't care about the extension .mod .
I recommend to make a National library file.
So please copy the contentents of all models from National into
one file Nat.lib. That's the same way LT has done it with its Ltc.lib.
You will then have your library file
C:ProgrammeLtcSwCADIIIlibsubPrivateNat.lib .


Part of the lm741.mod file:

*//////////////////////////////////////////////////////////
*LM741 OPERATIONAL AMPLIFIER MACRO-MODEL
*//////////////////////////////////////////////////////////
*
* connections: non-inverting input
* | inverting input
* | | positive power supply
* | | | negative power supply
* | | | | output
* | | | | |
* | | | | |
.SUBCKT LM741/NS 1 2 99 50 28
*
*Features:
*Improved performance over industry standards
....

The order of the functional pins is important for the coming symbol.
You are in luck here. Nearly all models of different vendors use
the same order. That means you can use an already existing symbol
from Linear Technolgoy.


1. Start LTSPICE

2. Start your Windows explorer and show the directory contents of
C:ProgrammeLtcSwCADIIIlibsymOpamps
Drag the symbol file Lt1013.asy to the LTSPICE program(window).
The symbol editor of LTSPICE now shows the symbol.

3. Make a new symbol by copying it. Still in the symbol editor press
File- >Save
Change LT1013.asy to Lm741.asy
Click up and down to the new folder
C:ProgrammeLtcSwCADIIIlibsymPrivate
Save the Lm741.asy here.

4. Now Edit- >Attributes->Edit Attributes
Replace the text Ltc.lib" with PrivateNat.lib or if you don't
want the library file then simply use Privatelm741.mod .

5. Replace both LT1013 with LM741/NS . This must be exactly the name
in the model file; see the line from that file above.
.SUBCKT LM741/NS 1 2 99 50 28

Finally your window looks like this:

Prefix X
SpiceModel PrivateNat.lib
Value LM741/NS
Value2 LM741/NS
Specline
Specline2
Descripion Whatever text you like

Press OK
File Save

6. Close LTSPICE !

7. Restart LTSPICE
File- > New Schematic

8. Click on Component or Edit- >Component
You should see your folder {private], click on it.
Now you see your symbol lm741 .
Click on it and place it to your schematic.

That's all you need.

Have fun with LTSPICE.
