LTspice: Getting it to use my subcircuit

  • Thread starter Mike Rocket J. Squirrel E
  • Start date
M

Mike Rocket J. Squirrel E

Guest
I have a power mosfet subcircuit that I wish to use. When I place
LTspice's PMOS symbol onto the schematic, it offers only a fairly short
list of devices to pick from, and no apparent way to enter the name of
the subcircuit I have. Where's it getting that selection of parts from?
Standard.mos seems to have a lot more devices than is being offered when
placing. In addition, they are models, not subcircuits.

How can I use my subcircuit with LTspice's PMOS symbol?

--
Mike "Rocket J Squirrel" Elliott
 
Just to explain -- I did read the Help file, and it says,

If you want to use a subcircuit, follow the following steps:

1. Change the "Prefix" attribute of the component instance of the
symbol to be an 'X'. Don't change the symbol, just the instances of
the symbol as a component on a schematic.

Can't figure out how to do that. The PMOS symbol seems to be some kinda
special symbol that does not allow editing.

Mike Rocket J. Squirrel Elliott wrote:

I have a power mosfet subcircuit that I wish to use. When I place
LTspice's PMOS symbol onto the schematic, it offers only a fairly short
list of devices to pick from, and no apparent way to enter the name of
the subcircuit I have. Where's it getting that selection of parts from?
Standard.mos seems to have a lot more devices than is being offered when
placing. In addition, they are models, not subcircuits.

How can I use my subcircuit with LTspice's PMOS symbol?
Click to expand...
--
Mike "Rocket J Squirrel" Elliott
 
Never mind -- I figured it out (myself!).

Opened the symbol in LTspice and changed the instance name from Mnnn to
X (it defaulted to "U" at that point) and saved it under a new name.

Then, when placing it on the schematic, the usual Component Attribute
Editor could be opened, and, well, the usual stuff could be done.

Something special about that "M" I figure.

Mike Rocket J. Squirrel Elliott
-------------------------------

Mike Rocket J. Squirrel Elliott wrote:

Just to explain -- I did read the Help file, and it says,

If you want to use a subcircuit, follow the following steps:

1. Change the "Prefix" attribute of the component
instance of the symbol to be an 'X'. Don't change the
symbol, just the instances of the symbol as a component on a
schematic.

Can't figure out how to do that. The PMOS symbol seems to be some kinda
special symbol that does not allow editing.

Mike Rocket J. Squirrel Elliott wrote:

I have a power mosfet subcircuit that I wish to use. When I place
LTspice's PMOS symbol onto the schematic, it offers only a fairly
short list of devices to pick from, and no apparent way to enter the
name of the subcircuit I have. Where's it getting that selection of
parts from? Standard.mos seems to have a lot more devices than is
being offered when placing. In addition, they are models, not
subcircuits.

How can I use my subcircuit with LTspice's PMOS symbol?
Click to expand...
--
Mike "Rocket J Squirrel" Elliott
 
----- Original Message -----
From: "Mike Rocket J. Squirrel Elliott"
<j.michael.elliottAT@REMOVETHEOBVIOUSadelphiaDOT.net>
Newsgroups: sci.electronics.cad
Sent: Saturday, November 08, 2003 3:02 AM
Subject: Re: LTspice: Getting it to use my subcircuit


Never mind -- I figured it out (myself!).

Opened the symbol in LTspice and changed the instance name from Mnnn to
X (it defaulted to "U" at that point) and saved it under a new name.

Then, when placing it on the schematic, the usual Component Attribute
Editor could be opened, and, well, the usual stuff could be done.

Something special about that "M" I figure.
Click to expand...
Hello Mike,
all the basic symbols(NPN, PNP, NMOS ...) for subcircuits are available
from the LTSPICE-Yahoo group. http://groups.yahoo.com/group/LTspice/
They are in the folder "Files>Lib>Sym>Universal Subcircuits" .

A more detailed explanation about symbol types in LTSPICE can be found
in the folder "Files->Tut->Symbol Types For Subcircuits".

I have a power mosfet subcircuit that I wish to use. When I place
LTspice's PMOS symbol onto the schematic, it offers only a fairly
short list of devices to pick from, and no apparent way to enter the
name of the subcircuit I have.
Click to expand...
The file standard.mos contains only direct mosfet models (.MODEL).

Where's it getting that selection of
parts from? Standard.mos seems to have a lot more devices than is
being offered when placing. In addition, they are models, not
subcircuits.
Click to expand...
I see all the types from the file in the selction window.
Have you added these extra models yourself?
Maybe you haven't done it exactly in the same way as the original models.

Best Regards
Helmut
 
On Sat, 8 Nov 2003 10:04:27 +0100, "Helmut Sennewald"
<HelmutSennewald@t-online.de> wrote:

----- Original Message -----
From: "Mike Rocket J. Squirrel Elliott"
j.michael.elliottAT@REMOVETHEOBVIOUSadelphiaDOT.net
Newsgroups: sci.electronics.cad
Sent: Saturday, November 08, 2003 3:02 AM
Subject: Re: LTspice: Getting it to use my subcircuit


Never mind -- I figured it out (myself!).

Opened the symbol in LTspice and changed the instance name from Mnnn to
X (it defaulted to "U" at that point) and saved it under a new name.

Then, when placing it on the schematic, the usual Component Attribute
Editor could be opened, and, well, the usual stuff could be done.

Something special about that "M" I figure.

Hello Mike,
all the basic symbols(NPN, PNP, NMOS ...) for subcircuits are available
from the LTSPICE-Yahoo group. http://groups.yahoo.com/group/LTspice/
They are in the folder "Files>Lib>Sym>Universal Subcircuits" .

A more detailed explanation about symbol types in LTSPICE can be found
in the folder "Files->Tut->Symbol Types For Subcircuits".


I have a power mosfet subcircuit that I wish to use. When I place
LTspice's PMOS symbol onto the schematic, it offers only a fairly
short list of devices to pick from, and no apparent way to enter the
name of the subcircuit I have.

The file standard.mos contains only direct mosfet models (.MODEL).

Where's it getting that selection of
parts from? Standard.mos seems to have a lot more devices than is
being offered when placing. In addition, they are models, not
subcircuits.

I see all the types from the file in the selction window.
Have you added these extra models yourself?
Maybe you haven't done it exactly in the same way as the original models.

Best Regards
Helmut
Click to expand...
PSpice Schematics allows meaningful reference designators Mxxx, Qxxx,
etc. on the schematic, yet uses subcircuit notation in the netlist
itself.

The reference designator converts, via the Template to:

X^@REFDES node1 node2 node3 node4 ModelName Params: ...

...Jim Thompson
--
| James E.Thompson, P.E. | mens |
| Analog Innovations, Inc. | et |
| Analog/Mixed-Signal ASIC's and Discrete Systems | manus |
| Phoenix, Arizona Voice:(480)460-2350 | |
| E-mail Address at Website Fax:(480)460-2142 | Brass Rat |
| http://www.analog-innovations.com | 1962 |

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

PSpice Schematics allows meaningful reference designators Mxxx, Qxxx,
etc. on the schematic, yet uses subcircuit notation in the netlist
itself.

The reference designator converts, via the Template to:

X^@REFDES node1 node2 node3 node4 ModelName Params: ...
Click to expand...
LTspice also allows you to name a component anything you
want, e.g., Q1 can be a subcircuit or a MOSFET, not just
just a bipolar transistor. It's the symbols' "Prefix"
attribute that determines how it netlists. This attribute
is similar to the first letter of the PSpice Schmatic's
"Template". However, in LTspice you can set the Prefix
attribute for an instance of a symbol on the schematic,
not just prefine it in the symbol creation, so the same
exact symbol can netlit as a subcirciut or any other
device you want. To edit the "Prefix" attribute, hold
down the control key and right click on the body of the
part on the schematic.

--Mike
 
Mike Engelhardt wrote:

[snip]

"Prefix" attribute, hold down the control key
and right click on the body of the part on the schematic.
Click to expand...
Oh for crying out loud. I use ctrl-right-click all the time to edit
component attributes. I have no explanation not involving spells, hexes
or simplicity why I didn't do it this time.

--
Mike "Rocket J Squirrel" Elliott
 
Helmut Sennewald wrote:

----- Original Message ----- From: "Mike Rocket J. Squirrel Elliott"
j.michael.elliottAT@REMOVETHEOBVIOUSadelphiaDOT.net> Newsgroups:
sci.electronics.cad Sent: Saturday, November 08, 2003 3:02 AM
Subject: Re: LTspice: Getting it to use my subcircuit




Hello Mike, all the basic symbols(NPN, PNP, NMOS ...) for subcircuits
are available from the LTSPICE-Yahoo group.
http://groups.yahoo.com/group/LTspice/ They are in the folder
"Files>Lib>Sym>Universal Subcircuits" .
Click to expand...
Hi Helmut -- I wasn't aware of that. Thank you!

A more detailed explanation about symbol types in LTSPICE can be
found in the folder "Files->Tut->Symbol Types For Subcircuits".
Click to expand...
I will join the group and look!

I have a power mosfet subcircuit that I wish to use. When I
place LTspice's PMOS symbol onto the schematic, it offers only
a fairly short list of devices to pick from, and no apparent
way to enter the name of the subcircuit I have.


The file standard.mos contains only direct mosfet models (.MODEL).
Click to expand...
I admit that it eludes me why there must be two ways to describe
components: subcircuits and models.

Where's it getting that selection of

parts from? Standard.mos seems to have a lot more devices than
is being offered when placing. In addition, they are models,
not subcircuits.

I see all the types from the file in the selction window. Have you
added these extra models yourself?

Maybe you haven't done it exactly in the same way as the original
models.
Click to expand...
I only have the one new MOSFET I need to use -- a 500V/2A P-channel
part. I use a standalone application from my old ISpice days:
Spicemodeler. It will create MOSFET (and other device) subcircuits from
data sheet information.

My question came from looking at the list of available parts that
LTspice offered when right-clicking (not Ctrl-right-clicking) on the
PMOS component. The standard.mos file contained many more parts than the
drop-down box showed. This, I think, was an accident -- a couple days
ago an interim version of LTspice suffered a crash and when I installed
the newest version, there were a few damaged files laying around. It's
all repaired now, with Mike's help, and the dropdown box agrees with
standard.mos.

At least I know enough to not add subcircuits to a file containing models!

--
Mike "Rocket J Squirrel" Elliott
 
On Sat, 08 Nov 2003 18:06:16 GMT, "Mike Rocket J. Squirrel Elliott"
<j.michael.elliottAT@REMOVETHEOBVIOUSadelphiaDOT.net> wrote:

[snip]
I admit that it eludes me why there must be two ways to describe
components: subcircuits and models.

[snip]
Click to expand...

GENERALLY, models describe *single* active devices such as BJTs,
MOSFETs, resistors, capacitors, etc.; subcircuits can have *multiple*
devices in them... for example you could make a whole schematic into a
subcircuit.

...Jim Thompson
--
| James E.Thompson, P.E. | mens |
| Analog Innovations, Inc. | et |
| Analog/Mixed-Signal ASIC's and Discrete Systems | manus |
| Phoenix, Arizona Voice:(480)460-2350 | |
| E-mail Address at Website Fax:(480)460-2142 | Brass Rat |
| http://www.analog-innovations.com | 1962 |

I love to cook with wine. Sometimes I even put it in the food.
 
Jim Thompson wrote:

On Sat, 08 Nov 2003 18:06:16 GMT, "Mike Rocket J. Squirrel Elliott"
j.michael.elliottAT@REMOVETHEOBVIOUSadelphiaDOT.net> wrote:

[snip]

I admit that it eludes me why there must be two ways to describe
components: subcircuits and models.


[snip]

GENERALLY, models describe *single* active devices such as BJTs,
MOSFETs, resistors, capacitors, etc.; subcircuits can have *multiple*
devices in them... for example you could make a whole schematic into a
subcircuit.
Click to expand...
This makes sense. Thanks.

--
Mike "Rocket J Squirrel" Elliott
 
You must log in or register to reply here.

Welcome to EDABoard.com

Sponsor

Back
Top