AB said:
OK, yes, I remember reading that. Of course, I thought it referred to
creating subcircuits for the purpose of circumventing the 60 component
per project limit.
Saying it that was is kinda like telling the astronauts that it's
going to get hard to breathe as they run out of oxygen:>:
I just installed LTSpice and I'm reading the help file now.
They don't talk about adding spice models either..I hope it's just
because I haven't gotten to that part yet.
Hello Art,
I posted an instruction a few weeks ago in this group. I have attached it
at the end of this message. There is also some info in the help pages I
think.
Sure hope I can add a Maxim laser driver chip and a tunnel diode:>:
It's no problem if you have a model or at least know how to model it.
Maybe I should have asked on this list BEFORE investing the time is
LTSpice!
There is a LTSPICE user group for support too.
http://groups.yahoo.com/group/LTspice/
Best Regards
Helmut
Joe said:
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:\Programme\Ltc\SwCADIII\lib\sub\Private
For the symbols:
C:\Programme\Ltc\SwCADIII\lib\sym\Private
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:\Programme\Ltc\SwCADIII\lib\sub\Private
We have then C:\Programme\Ltc\SwCADIII\lib\sub\Private\lm741.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:\Programme\Ltc\SwCADIII\lib\sub\Private\Nat.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:\Programme\Ltc\SwCADIII\lib\sym\Opamps
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:\Programme\Ltc\SwCADIII\lib\sym\Private
Save the Lm741.asy here.
4. Now Edit->Attributes->Edit Attributes
Replace the text Ltc.lib" with Private\Nat.lib or if you don't
want the library file then simply use Private\lm741.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 Private\Nat.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.
One of your other questions was about HSPICE and PSPICE models.
You should prefer PSPICE models, because LTSPICE is most compatible to that.
This is the user's group of LTSPICE.
http://groups.yahoo.com/group/LTspice
Best Regards
Helmut