CircuitMaker and Spice... How to add chips to Spice?

[AB]

How do I add a spice model for a 74HC14 inverter???? I need the HC
variant, so I can't use the 7414 model that comes with my Spice.

I am running CircuitMaker, Student version. The docs say it uses
Berkley Spice.

I found the models folder, and it contains .mod, .lib and .sub
(subcircuits, which I am not allowed to use with my Student version).

I read the help file, but it's all Greek to me.

I'm new at Spice and I'm still learning:>:

Can someone give me a push in the right direction????

I have a spec sheet for the 74HC14.

Thanks,

Art

 

[Chaos Master]

AB screamed:

How do I add a spice model for a 74HC14 inverter???? I need the HC
variant, so I can't use the 7414 model that comes with my Spice.

I am running CircuitMaker, Student version. The docs say it uses
Berkley Spice.

CM Student doesn't allow you to add new models.
The help file says to use the Macro menu (that isn't avaliable in the
Student version). I once tried to contact the support(they claim they
give support via email for users of the Student version), but the email
bounced.

--
E-mail address is fake. Please reply to the group!

 

[AB]

On Sun, 31 Aug 2003 17:32:51 -0300, Chaos Master
<raw_chaos@brasnet.org> wrote:

AB screamed:
How do I add a spice model for a 74HC14 inverter???? I need the HC
variant, so I can't use the 7414 model that comes with my Spice.

I am running CircuitMaker, Student version. The docs say it uses
Berkley Spice.

CM Student doesn't allow you to add new models.

Oh, that's just swell! Sure wish they told me that when I downloaded
it!

Thanks for passing the word, I appreciate the info.

AB

 

[AB]

They tell you, in some form: "Symbol editor and Macro feature disabled".
But that's a bit strange. When I dl'ed it, I thought Macro feature
refered to creating your own subcircuits.

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.

Sure hope I can add a Maxim laser driver chip and a tunnel diode:>:

Maybe I should have asked on this list BEFORE investing the time is
LTSpice!

Regards,

Art

 

[Active8]

In article <4f15lvgnlminfavml1bgqug1nd57r63m7q@4ax.com>,
artky1k@uninets.net says...

They tell you, in some form: "Symbol editor and Macro feature disabled".
But that's a bit strange. When I dl'ed it, I thought Macro feature
refered to creating your own subcircuits.




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.

Sure hope I can add a Maxim laser driver chip and a tunnel diode:>:

Maybe I should have asked on this list BEFORE investing the time is
LTSpice!

Regards,

Art
actually, LTSpice is damned good and if it's possible to do what you

want and it's not in the help, you'll most likely get an answer here.

mike

 

[Chaos Master]

Active8 screamed:

In article <4f15lvgnlminfavml1bgqug1nd57r63m7q@4ax.com>,
artky1k@uninets.net says...

actually, LTSpice is damned good and if it's possible to do what you
want and it's not in the help, you'll most likely get an answer here.
Exactly. The help isn't sooooooooooo good.

--
E-mail address is fake. Please reply to the group!

 

[Helmut Sennewald]

"AB" <artky1k@uninets.net> schrieb im Newsbeitrag
news:4f15lvgnlminfavml1bgqug1nd57r63m7q@4ax.com...

They tell you, in some form: "Symbol editor and Macro feature disabled".
But that's a bit strange. When I dl'ed it, I thought Macro feature
refered to creating your own subcircuits.




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" <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]

AB wrote:

How do I add a spice model for a 74HC14 inverter???? I need the HC
variant, so I can't use the 7414 model that comes with my Spice.

I am running CircuitMaker, Student version. The docs say it uses
Berkley Spice.

I found the models folder, and it contains .mod, .lib and .sub
(subcircuits, which I am not allowed to use with my Student version).

I read the help file, but it's all Greek to me.

I'm new at Spice and I'm still learning:>:

Can someone give me a push in the right direction????

I have a spec sheet for the 74HC14.

SuperSpice,http://www.anasoft.co.uk installs with a generic cmos
inverter which is pretty much equivalent to the hc series. Secondly, its
a simple drag drop to add new model files. The demo only limits save and
netlsit size. Everything else is fully enabled.

In addition, in the demo version, if you use the schematic hierarchy,
you can get 30 top level blocks, and 25 components per block giving a
total of around 750 components. There is no limit to the size of any
..subckt.

Kevin Aylward
sales@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.

 

[AB]

Thanks to all.

I just signed up for the LTSpice mailing list as Helmut suggested.

I follow most of the procedure Helmut gave for adding models and I'll
give it a try for the 74HC14.

I played yesterdsay for awhile looking for an LT chip that would do my
power supply needs, but they are real power hogs compared to Maxim
IC's. I hope I can get a Maxim IC into this Spice somehow!

I might try SuperSpice too. I loooked at it day before yesterday, but
decided to try LTSPice first.

Do any of these programs come with complete spice library's ordoes
anyone have spice models that can be installed using a zip file (so
5000 or more models could be added in a single shot)??

I also have a crippleware version of Orcad Capture with PSpice. But,
as far as I can tell, it does not include any Spice models at all! Not
sure about that, but I did do some of the tutorial and it is
complicated, hard to learn and the full version sells for big bux.

Have a great day and a better tomorrow.

Art

On Mon, 1 Sep 2003 07:32:25 +0200, "Helmut Sennewald"
<HelmutSennewald@t-online.de> wrote:

"AB" <artky1k@uninets.net> schrieb im Newsbeitrag
news:4f15lvgnlminfavml1bgqug1nd57r63m7q@4ax.com...

They tell you, in some form: "Symbol editor and Macro feature disabled".
But that's a bit strange. When I dl'ed it, I thought Macro feature
refered to creating your own subcircuits.




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" <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

 

[AB]

As I noted, in my other post, in SuperSpice, you simply drag drop such a
file containing models and your done as far as adding in the
models/subckts. Spice .models, will automatically have the correct
symbols attached to them, .subckt can be GUI click attached to existing
symbols. There is also a simple GUI auto generate of new block symbols
for .subckt. that have no appropriate symbol already existing.

Kevin Aylward
salesEXTRACT@anasoft.co.uk
http://www.anasoft.co.uk

Kevin,

I'm a small potato and can't afford the price for SuperSpice. If I ran
a business, I'd be happy to pay the price for it. But, I'm a hobbyist
and just want to putz and learn Spice so I can use it on a very
limited number of projects.

How many spice models come with it (the evaluation version)? If it's
really that easy, I wonder why you (and other spice vendors) don't
assemble the models and distribute them with the software?

It appears that you use Berkley Spice, which means custom models that
aren't drag and drop from a pspice model file?? I'm having a tough
time with all of this, it's all so new to me.

Please excuse the stupicd questions.

Art

 

[Jim Thompson]

On Mon, 01 Sep 2003 18:14:05 -0400, AB <artky1k@uninets.net> wrote:

As I noted, in my other post, in SuperSpice, you simply drag drop such a
file containing models and your done as far as adding in the
models/subckts. Spice .models, will automatically have the correct
symbols attached to them, .subckt can be GUI click attached to existing
symbols. There is also a simple GUI auto generate of new block symbols
for .subckt. that have no appropriate symbol already existing.

Kevin Aylward
salesEXTRACT@anasoft.co.uk
http://www.anasoft.co.uk

Kevin,

I'm a small potato and can't afford the price for SuperSpice. If I ran
a business, I'd be happy to pay the price for it. But, I'm a hobbyist
and just want to putz and learn Spice so I can use it on a very
limited number of projects.

How many spice models come with it (the evaluation version)? If it's
really that easy, I wonder why you (and other spice vendors) don't
assemble the models and distribute them with the software?

It appears that you use Berkley Spice, which means custom models that
aren't drag and drop from a pspice model file?? I'm having a tough
time with all of this, it's all so new to me.

Please excuse the stupicd questions.

Art

I know not of CircuitMaker, but LTSpice, SuperSpice, PSpice and most
other legitimate Spices will all run the same models (although LTSpice
has some models of their proprietary product line encoded so they
won't work elsewhere).

...Jim Thompson
--
| James E.Thompson, P.E. | mens |
| Analog Innovations, Inc. | et |
| Analog/Mixed-Signal ASIC's and Discrete Systems | manus |
| Phoenix, Arizona Voice480)460-2350 | |
| E-mail Address at Website Fax480)460-2142 | Brass Rat |
| http://www.analog-innovations.com | 1962 |

I love to cook with wine. Sometimes I even put it in the food.

 

[AB]

SuperSpice,http://www.anasoft.co.uk installs with a generic cmos
inverter which is pretty much equivalent to the hc series. Secondly, its
a simple drag drop to add new model files. The demo only limits save and
netlsit size. Everything else is fully enabled.

In addition, in the demo version, if you use the schematic hierarchy,
you can get 30 top level blocks, and 25 components per block giving a
total of around 750 components. There is no limit to the size of any
.subckt.

OK Kevin, thanks,

I downloaded it earlier this evening and I must say you have the user
interface that is GREAT!

I need a 74HC14 because of its low power consumption, because of its
enhanced drive ability (source/sink 25 ma) and because it is a Schmitt
trigger and I'm using it in an analog circuit with slow and variable
speed edges. I need some precision in prop delay times too, which
can't come from a generic.

A generic one won't do.

I look forward to dragging and dropping to add new models!

I just fired it up a few minutes ago and found my way to the examples
and ran a few. Looks great.

Now, I gotta figure out how to make it do my circuit!

Art

 

[Chaos Master]

Jim Thompson screamed:

On Mon, 01 Sep 2003 18:14:05 -0400, AB <artky1k@uninets.net> wrote:
I know not of CircuitMaker, but LTSpice, SuperSpice, PSpice and most
other legitimate Spices will all run the same models (although LTSpice
has some models of their proprietary product line encoded so they
won't work elsewhere).

Some "older" SPICE programs will not run models based on behavioral
modelling. CircuitMaker is one of those.


--
E-mail address is fake. Please reply to the group!

 

[Kevin Aylward]

Chaos Master wrote:

Jim Thompson screamed:
On Mon, 01 Sep 2003 18:14:05 -0400, AB <artky1k@uninets.net> wrote:
I know not of CircuitMaker, but LTSpice, SuperSpice, PSpice and most
other legitimate Spices will all run the same models (although
LTSpice has some models of their proprietary product line encoded so
they won't work elsewhere).

Some "older" SPICE programs will not run models based on behavioral
modelling. CircuitMaker is one of those.

The latest CM, uses XSpice, so should run behavioural models. However,
the XSpice syntax is a little different from PSpice. Some XSpice based
products do the conversion automatically. I do this in SS, with just a
couple of exceptions. e.g. I have not gotten around to accepting
pow(x,y), XSpice wants x^y.

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.

 

[Kevin Aylward]

AB wrote:

As I noted, in my other post, in SuperSpice, you simply drag drop
such a file containing models and your done as far as adding in the
models/subckts. Spice .models, will automatically have the correct
symbols attached to them, .subckt can be GUI click attached to
existing symbols. There is also a simple GUI auto generate of new
block symbols for .subckt. that have no appropriate symbol already
existing.

Kevin,

I'm a small potato and can't afford the price for SuperSpice. If I ran
a business, I'd be happy to pay the price for it. But, I'm a hobbyist
and just want to putz and learn Spice so I can use it on a very
limited number of projects.

I will agree that, despite, in my view, a less then perfect gui, LTSpice
is a very good option. It is fast and converges well. It is actually
usable. Many commercial spices, are just about impossible to even probe
the signals. e.g. floating graph windows that always stay on top of the
schematic!

How many spice models come with it (the evaluation version)?

1000's....

If it's
really that easy,

Not for all spices. A lot of them require some fiddling about and
restarts etc.

I wonder why you (and other spice vendors) don't
assemble the models and distribute them with the software?

Well, for the most part, we do. I would say 99% of spice vendor supplied
models come from the manufactures. However, many spices have all sorts
of propriety data bases restricting access. SS doesn't do this. The
models stay in a simple text file.

In SS case, I try and limit my download file size. It is about 5Meg, and
is fully complete, only requiring a password file to turn into the full
version. Many Spices are 50MB. In adition, although I have included a
lot of model files, they don't all get loaded into the file browser, by
default.

It appears that you use Berkley Spice, which means custom models that
aren't drag and drop from a pspice model file??

PSpice is "basically" standard spice, but it does have some syntax
changes and some additional bits and bobs. By far the majority of PSpice
models work directly in Spice3/XSpice. Some need a few simple changes. I
do most of them automatically in SS.


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.

 

[Kevin Aylward]

AB wrote:

SuperSpice,http://www.anasoft.co.uk installs with a generic cmos
inverter which is pretty much equivalent to the hc series. Secondly,
its a simple drag drop to add new model files. The demo only limits
save and netlsit size. Everything else is fully enabled.

In addition, in the demo version, if you use the schematic hierarchy,
you can get 30 top level blocks, and 25 components per block giving
a total of around 750 components. There is no limit to the size of
any .subckt.


OK Kevin, thanks,

I downloaded it earlier this evening and I must say you have the user
interface that is GREAT!

Thanks. As I often point out, I'm only a Software hack. My profession,
and has been for the last 20 odd years, is as an analogue design
engineer, and one that ould not afford ones own copy of PSpice around 6
years ago. we aren't all as wealthy as Jim Thompson.

I need a 74HC14 because of its low power consumption, because of its
enhanced drive ability (source/sink 25 ma) and because it is a Schmitt
trigger and I'm using it in an analog circuit with slow and variable
speed edges. I need some precision in prop delay times too, which
can't come from a generic.

A generic one won't do.

My generic versions, are a reasonable approximation to the real device,
which a digital model isn't in way.

The "digital" models in the "AnalogDigital" model folder are all
transistor level cmos versions. They can be copied and modified so that
they model the speed and drive of a particular device type better. The
capacitances of the Schmitt is a bit high for hc, it speed is set around
the 4000 speed.

The hc4066 analogue switch should be fairly accurate.

I look forward to dragging and dropping to add new models!

I just fired it up a few minutes ago and found my way to the examples
and ran a few. Looks great.

The examples are designed to show all the main features. Its worth
running them all. Note that a couple of the schematics are not directly
runable, as they are called from a top-level schematic.


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.

 

[Kevin Aylward]

Terry Pinnell wrote:

Chaos Master <raw_chaos@brasnet.org> wrote:

Jim Thompson screamed:
On Mon, 01 Sep 2003 18:14:05 -0400, AB <artky1k@uninets.net> wrote:
I know not of CircuitMaker, but LTSpice, SuperSpice, PSpice and most
other legitimate Spices will all run the same models (although
LTSpice has some models of their proprietary product line encoded
so they won't work elsewhere).

Some "older" SPICE programs will not run models based on behavioral
modelling. CircuitMaker is one of those.

That's news to me if true. I'm pretty sure CircuitMaker 2000 using
Berkeley Spice3f5/XSpice handles it. Perhaps I don't grasp the
definition. Could you amplify on what you mean by'behavioural
modelling', and an example of one that CM can't run please?

"behavioural" is just a fancy name for "generic equations".

b1 1 0 v=v(1,2)*log(V(3,4)) + 1

Is a "behavioural" description in XSpice, so CM should certainly be able
to run it. Likewise, with Laplace transforms.

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]

"Kevin Aylward" <kevin@anasoft.co.uk> wrote:

"behavioural" is just a fancy name for "generic equations".

b1 1 0 v=v(1,2)*log(V(3,4)) + 1

Is a "behavioural" description in XSpice, so CM should certainly be able
to run it. Likewise, with Laplace transforms.

OK, thanks.In that case I'm doubly sure Chaos master was mistaken on
that point.

--
Terry Pinnell
Hobbyist, West Sussex, UK

 

[Chaos Master]

Terry Pinnell screamed:

OK, thanks.In that case I'm doubly sure Chaos master was mistaken on
that point.

I was mistaken. Sorry. I used CM 2000 demo, just for testing.
--
E-mail address is fake. Please reply to the group!