Need help with LTSPICE library

[Joe]

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??

TIA,

Joe

 

[Joe]

"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

 

[Kevin Aylward]

Joe wrote:

"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

The Spice2, Spice3 format is understood by just about all simulators, so
a basic model usually runs in all. However, PSpice and HSpice have some
extra stuff that might cause problems if their extensions are used.

. 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??

See above. There is the a standard html Berkley manual in my SuperSpice
install.

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,

This prompted me to address my own SuperSpice 555 model. It had some
convergence problems. My latest update:

2 Implemented a new 555 Timer .subckt model with much better convergence
properties. The Example LM555.sss has been updated. This example now has
a 555 set to Astable mode, driving a 555 set to Monostable mode, but
with its control voltage modulated to form a PWM.

It runs fine in SS with this example, and should run ok in any of the
XSpice based simulators, e.g., EWB, Circuit Maker, Visual Spice, Tina,
TopSpice. However, there seems to be an issue in LTSpice, it runs at a
snails pace.

Ah... just played with LTSpice a bit while writing this... quite
strange. It wants a default of abstol=10p, then it zooms off at about
twice the speed. I modified the basic xspice engine default to 10p from
1p, so I dont have this in my .options line. I found 10p to be a bettter
defualt for most circuits.

Kevin Aylward
salesEXTRACT@anasoft.co.uk
http://www.anasoft.co.uk
SuperSpice, a very affordable Mixed-Mode
Windows Simulator with Schematic Capture,
Waveform Display, FFT's and Filter Design.
**********

 

[Helmut Sennewald]

"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:\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

 

[Kevin Aylward]

Joe wrote:

"Helmut Sennewald" <HelmutSennewald@t-online.de> wrote in message


Helmut,
Thank you very much for the info. I followed all the steps and just
simulated the 741 to test everything. It seems to work fine. I would
like to know what all those numbers mean in the model. Is there a
source I can go to in order to find out what all the numbers mean?
I also noticed that when I ran the simulation, and was probing the
pins, the pin numbers seemed to correspond to the first line in the
.subckt definition:
1,2,99,50,28 . The actual pins are 3,2,7,4,6 on the 8 pin dip.
Is this the standard definition you mentioned above?
I also signed up for the ltspice group on yahoogroups.

Thank you again for the great info, I am off and running now!

Standard Spice manual http://www.anasoft.co.uk/Spice3F5Manual.html

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

 

[Terry Pinnell]

"Helmut Sennewald" <HelmutSennewald@t-online.de> wrote:

Hello Joe,
here is the fastest route to your models in LTSPICE.
[snipped comprehensive step-by-step procedure]

Nice one, Helmut!

I wish I had such a clear and succinct guide for CircuitMaker <g>.

--
Terry Pinnell
Hobbyist, West Sussex, UK

 

[Helmut Sennewald]

"Joe" <nuisancewildlife@nospamearthlink.net> schrieb im Newsbeitrag
news:F7X_a.20545$vo2.15298@newsread1.news.atl.earthlink.net...

"Helmut Sennewald" <HelmutSennewald@t-online.de> wrote in message
news:bhgpcd$vgc$03$1@news.t-online.com...
"Joe" <nuisancewildlife@nospamearthlink.net> schrieb im Newsbeitrag
news:uAA_a.13045$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:\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

Helmut,
Thank you very much for the info. I followed all the steps and just
simulated the 741 to test everything. It seems to work fine. I would like
to
know what all those numbers mean in the model. Is there a source I can go
to
in order to find out what all the numbers mean?

Hello Joe,
this is just SPICE syntax. Kevin has already given you a link to a
SPICE manual. Take a look into it.
Every node of your circuit has a unique number. You are free to
number it except number 0 which is the common node. Every circuit
needs a DC path in some way to node 0. That's wy SPICE will fail
normally if you have no GND symbol on your schematic.
If you use a schematic then LTSPICE number the nodes for you.
You can see it after a simulalation run with
View-> SPICE netlist
Spice interpreters these days allows also names insted of numbers.
Example: R100 23 34 1k
R101 inp rc 2k

I also noticed that when I ran the simulation, and was probing the pins,
the
pin numbers seemed to correspond to the first line in the .subckt
definition:
1,2,99,50,28 . The actual pins are 3,2,7,4,6 on the 8 pin dip.
Is this the standard definition you mentioned above?

The physical pins of your device has nothing to do with the pin order
in the sub-circuit. Somebody just started to use the order
non-inv. invert. pos.supp. ...... . All the other people
have followed for compatibility reason.

* connections: non-inverting input
* | inverting input
* | | positive power supply
* | | | negative power supply
* | | | | output
* | | | | |
* | | | | |
.SUBCKT LM741/NS 1 2 99 50 28

Best Regards
Helmut

 

[Joe]

"Kevin Aylward" <kevin@anasoft.co.uk> wrote in message
news:0I__a.21$xV3.19@newsfep3-gui.server.ntli.net...

Joe wrote:
"Helmut Sennewald" <HelmutSennewald@t-online.de> wrote in message


Helmut,
Thank you very much for the info. I followed all the steps and just
simulated the 741 to test everything. It seems to work fine. I would
like to know what all those numbers mean in the model. Is there a
source I can go to in order to find out what all the numbers mean?
I also noticed that when I ran the simulation, and was probing the
pins, the pin numbers seemed to correspond to the first line in the
.subckt definition:
1,2,99,50,28 . The actual pins are 3,2,7,4,6 on the 8 pin dip.
Is this the standard definition you mentioned above?
I also signed up for the ltspice group on yahoogroups.

Thank you again for the great info, I am off and running now!


Standard Spice manual http://www.anasoft.co.uk/Spice3F5Manual.html

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

Thank you Kevin, I downloaded the spice manual and I have started reading
it. The 741 subckt has a lot of R's and C's in it, and they are numbered
(ieR1, R2, etc.). Is R always a resistor, and C always a capacitor? These
occur at the beginning of each line in the model definition. If so, it looks
like this model is broken down to a bunch of resistors, caps , current and
voltage sources. Is that basically how these devices are modelled?

Joe

 

[Joe]

"Helmut Sennewald" <HelmutSennewald@t-online.de> wrote in message
news:bhi6si$q3k$06$1@news.t-online.com...

Helmut,
Thank you very much for the info. I followed all the steps and just
simulated the 741 to test everything. It seems to work fine. I would
like
to
know what all those numbers mean in the model. Is there a source I can
go
to
in order to find out what all the numbers mean?

Hello Joe,
this is just SPICE syntax. Kevin has already given you a link to a
SPICE manual. Take a look into it.
Every node of your circuit has a unique number. You are free to
number it except number 0 which is the common node. Every circuit
needs a DC path in some way to node 0. That's wy SPICE will fail
normally if you have no GND symbol on your schematic.
If you use a schematic then LTSPICE number the nodes for you.
You can see it after a simulalation run with
View-> SPICE netlist
Spice interpreters these days allows also names insted of numbers.
Example: R100 23 34 1k
R101 inp rc 2k

I also noticed that when I ran the simulation, and was probing the pins,
the
pin numbers seemed to correspond to the first line in the .subckt
definition:
1,2,99,50,28 . The actual pins are 3,2,7,4,6 on the 8 pin dip.
Is this the standard definition you mentioned above?

The physical pins of your device has nothing to do with the pin order
in the sub-circuit. Somebody just started to use the order
non-inv. invert. pos.supp. ...... . All the other people
have followed for compatibility reason.

* connections: non-inverting input
* | inverting input
* | | positive power supply
* | | | negative power supply
* | | | | output
* | | | | |
* | | | | |
.SUBCKT LM741/NS 1 2 99 50 28


Best Regards
Helmut

Thanks for explaining that. I am sure I will have many more questions as I
delve into the spice manual, and now that I know how to look at the spice
netlist. Is this the best forum for questions or should I post to the
LTSPICE group on yahoo?, or both?

Joe

PS I am having fun with this, actually, now that it is starting to make
sense)

 

[Helmut Sennewald]

"Joe" <nuisancewildlife@nospamearthlink.net> schrieb im Newsbeitrag
news:Fqf%a.16242$BC2.16013@newsread2.news.atl.earthlink.net...

"Helmut Sennewald" <HelmutSennewald@t-online.de> wrote in message
news:bhi6si$q3k$06$1@news.t-online.com...

.....

Thanks for explaining that. I am sure I will have many more questions as I
delve into the spice manual, and now that I know how to look at the spice
netlist. Is this the best forum for questions or should I post to the
LTSPICE group on yahoo?, or both?

Hello Joe,
I would post general SPICE questions into this group and very
LTSPICE specific questions to the LTSPICE-YAHOO group.
The LTSPICE-Yahoo group is a forum to share files too.
That can't be done with this group here.

The advantage of the sci.electronics.cad group is that you
reach people using different SPICE programs. None of the SPICE
implementations is best in all features.

Many people interested in LTSPICE read in both groups anyway.

Best Regards
Helmut


This is the user's group of LTSPICE.
http://groups.yahoo.com/group/LTspice

 

[Kevin Aylward]

Joe wrote:

"Kevin Aylward" <kevin@anasoft.co.uk> wrote in message
news:0I__a.21$xV3.19@newsfep3-gui.server.ntli.net...
Joe wrote:
"Helmut Sennewald" <HelmutSennewald@t-online.de> wrote in message


Helmut,
Thank you very much for the info. I followed all the steps and just
simulated the 741 to test everything. It seems to work fine. I would
like to know what all those numbers mean in the model. Is there a
source I can go to in order to find out what all the numbers mean?
I also noticed that when I ran the simulation, and was probing the
pins, the pin numbers seemed to correspond to the first line in the
.subckt definition:
1,2,99,50,28 . The actual pins are 3,2,7,4,6 on the 8 pin dip.
Is this the standard definition you mentioned above?
I also signed up for the ltspice group on yahoogroups.

Thank you again for the great info, I am off and running now!


Standard Spice manual http://www.anasoft.co.uk/Spice3F5Manual.html

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


Thank you Kevin, I downloaded the spice manual and I have started
reading it. The 741 subckt has a lot of R's and C's in it, and they
are numbered (ieR1, R2, etc.). Is R always a resistor, and C always a
capacitor?

Yes and Yes.

These occur at the beginning of each line in the model
definition. If so, it looks like this model is broken down to a bunch
of resistors, caps , current and voltage sources. Is that basically
how these devices are modelled?

Yes.

As I have prior noted, in SuperSpice, you can draw a schematic for the
model, and have the ".subckt" model text automatically generated. This
way you dont need to know anything about the spice syntax at all. I use
this method to make all my bigger models like PWM, current mode
controllers etc. Its much easier to probe debug the schematic version
than a text version.

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

 

[Joe]

"Kevin Aylward" <kevin@anasoft.co.uk> wrote in message
news:BUm%a.21$0V2.55825@newsfep1-win.server.ntli.net...

Thank you Kevin, I downloaded the spice manual and I have started
reading it. The 741 subckt has a lot of R's and C's in it, and they
are numbered (ieR1, R2, etc.). Is R always a resistor, and C always a
capacitor?

Yes and Yes.

These occur at the beginning of each line in the model
definition. If so, it looks like this model is broken down to a bunch
of resistors, caps , current and voltage sources. Is that basically
how these devices are modelled?


Yes.

As I have prior noted, in SuperSpice, you can draw a schematic for the
model, and have the ".subckt" model text automatically generated. This
way you dont need to know anything about the spice syntax at all. I use
this method to make all my bigger models like PWM, current mode
controllers etc. Its much easier to probe debug the schematic version
than a text version.

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

Ok, staying with the LM741 model. There is a transistor level schematic of
the LM 741 in the 'educational' folder of the LTSPICE directory. When I run
it, and look at the spice net list, I get a .asc file which I can then print
with notepad. I did that, but it doesnt look anything like the model I
downloaded from National. There are a lot of nodes and the pins are
different in the netlist. I am not sure how I could convert it to a .subckt
and then just use it as a model as I did with the national version. Looking
in the spice manual, I can see that it is related, but I seem to be missing
something that links the net list, and circuit description with the models
and subcircuits.

It seems like it would be a lot easier to do it that way, but I am not sure
if the spice net list is the same as a .subckt in LTSPICE.

Joe

 

[Mike Engelhardt]

Joe,

Ok, staying with the LM741 model. There is a transistor level schematic of
the LM 741 in the 'educational' folder of the LTSPICE directory. When I
run
it, and look at the spice net list, I get a .asc file which I can then
print
with notepad. I did that, but it doesnt look anything like the model I
downloaded from National. There are a lot of nodes and the pins are
different in the netlist. I am not sure how I could convert it to a
..subckt
and then just use it as a model as I did with the national version.
Looking
in the spice manual, I can see that it is related, but I seem to be
missing
something that links the net list, and circuit description with the models
and subcircuits.

It seems like it would be a lot easier to do it that way, but I am not
sure
if the spice net list is the same as a .subckt in LTSPICE.

The LT741 schematic isn't so much a macro model of 741, but the actual
transistor-level schematic of the IC. If you want to run it as the model
of a 741, the easiest way is to call it as schematic in a hierarchical
circuit. See the appropriate sections of the help to see how to do this.

--Mike

 

[Kevin Aylward]

Helmut Sennewald wrote:

"Joe" <nuisancewildlife@nospamearthlink.net> schrieb im Newsbeitrag
news:ZFu%a.25700$vo2.12708@newsread1.news.atl.earthlink.net...

"Kevin Aylward" <kevin@anasoft.co.uk> wrote in message
news:BUm%a.21$0V2.55825@newsfep1-win.server.ntli.net...



6. I have made the lines with *--- to comment lines.
You can remove those lines as well es every other line starting
with an * . The the line .end have to be replaced by .ends.
Every subcircuit must end with the .ends line.



The modified netlist.
Changed lines:
added .SUBCKT LM741 3 2 7 4 6
added .ends
removed
*---.model NPN NPN
*---.model PNP PNP
*---.lib F:\PROGRAMME\LTC\SWCADIII\lib\cmp\standard.bjt
*---.backanno
*---.end

I think its worth pointing out that in general, one does not want to
remove ".model" lines. Unless its a default model, there is no way that
an arbitrary simulator is going to include the correct model. It needs
to be specified in the ".subckt"

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