How to add .SPI file to LTSpice library?

M

Michael Noone

Guest
Hi - I'd like to add a model for the International Rectifier IRFBG20
(http://ec.irf.com/v6/en/US/adirect/ir?
cmd=catProductDetailFrame&productID=IRFBG20:) to LTSpice. On the page
linked to there is a spice file with a .SPI extension. I looked through the
LTSpice help file and they said that if it is not a model (and I'm assuming
it's not, as the file begins with ".SUBCKT" though there are a couple
".MODEL" in there as well) you have to follow a number of steps to add it.
I couldn't even get past the first step:

"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. You can access this attribute by holding down
the control key and right clicking on the body of the component."

as I couldn't find the prefix attribute in the .spi file (I'm assuming
that's where I look for it?)

So - can anybody help me? If you can't tell - I'm VERY new to Spice. Thanks
so much!

-Michael J. Noone
 
On Thu, 31 Mar 2005 21:17:50 GMT, Michael Noone
<mnoone.uiuc.edu@127.0.0.1> wrote:

Hi - I'd like to add a model for the International Rectifier IRFBG20
(http://ec.irf.com/v6/en/US/adirect/ir?
cmd=catProductDetailFrame&productID=IRFBG20:) to LTSpice. On the page
linked to there is a spice file with a .SPI extension. I looked through the
LTSpice help file and they said that if it is not a model (and I'm assuming
it's not, as the file begins with ".SUBCKT" though there are a couple
".MODEL" in there as well) you have to follow a number of steps to add it.
I couldn't even get past the first step:

"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. You can access this attribute by holding down
the control key and right clicking on the body of the component."

as I couldn't find the prefix attribute in the .spi file (I'm assuming
that's where I look for it?)

So - can anybody help me? If you can't tell - I'm VERY new to Spice. Thanks
so much!

-Michael J. Noone
Click to expand...
You're mixing up "declaration" and "instantiation" of subcircuits, but
I'll leave it to Mike to detail it for you in LTspice.

...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.
 
"Michael Noone" <mnoone.uiuc.edu@127.0.0.1> schrieb im Newsbeitrag
news:Xns962A9B97F4565mnooneuiucedu127001@204.127.204.17...
Hi - I'd like to add a model for the International Rectifier IRFBG20
(http://ec.irf.com/v6/en/US/adirect/ir?
cmd=catProductDetailFrame&productID=IRFBG20:) to LTSpice. On the page
linked to there is a spice file with a .SPI extension. I looked through
the
LTSpice help file and they said that if it is not a model (and I'm
assuming
it's not, as the file begins with ".SUBCKT" though there are a couple
".MODEL" in there as well) you have to follow a number of steps to add it.
I couldn't even get past the first step:

"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. You can access this attribute by holding down
the control key and right clicking on the body of the component."

as I couldn't find the prefix attribute in the .spi file (I'm assuming
that's where I look for it?)
Click to expand...
Hello Michael,
an instance is a symbol after it has been placed on the schematic.
You could also say, a symbol becomes an instance after it's placed
on the schematic.
Don't touch the .spi file. It is ok and there is nothing to
change there. The filename or the extension of the filename has no
special meaning in LTspice. You can name the model file
'michael.noone' if you like.
This line have to be added(=placed) on the schematic.
..include IRFBG20.spi

The prefix has to be changed on the instance in the schematic.
The other chance is using a symbol which is already prepared
for this. It simply already has the prefix X instead of the
original prefix MN. A lot of such symbols for subcircuits
are in the Files area of the LTspice Yahoo group.

So - can anybody help me? If you can't tell - I'm VERY new to Spice.
Thanks
so much!

-Michael J. Noone
Click to expand...
Please try on the instance(=symbol on the schematic).
I have added a complete example at the end of this message.
Please try it too.

Best Regards,
Helmut

Ltspice/SwitcherCADIII is free of charge.
It can be downloaded from www.linear.com

The user group: www.groups.yahoo.com/LTspice


The example discussed above:
----------------------------
Put the text below into a file named IRFBG20_test.asc,
then open it with LTspice and press RUN.
Please keep the model file IRFBG20.spi in the same folder
as the schematic(.asc).


Version 4
SHEET 1 1512 988
WIRE -448 272 -448 240
WIRE -448 400 -448 352
WIRE -448 432 -448 400
WIRE -304 240 -448 240
WIRE -256 160 -256 128
WIRE -256 400 -448 400
WIRE -256 400 -256 256
WIRE -32 128 -256 128
WIRE -32 208 -32 128
WIRE -32 400 -256 400
WIRE -32 400 -32 288
FLAG -448 432 0
SYMBOL voltage -448 256 R0
SYMATTR InstName V1
SYMATTR Value 0
SYMBOL voltage -32 192 R0
SYMATTR InstName V2
SYMATTR Value 10
SYMBOL nmos -304 160 R0
SYMATTR InstName M1
SYMATTR Value IRFBG20
SYMATTR Prefix X
TEXT -448 16 Left 0 !.dc V2 0 15 0.01 V1 4 6 1
TEXT -448 64 Left 0 !.include IRFBG20.spi
 
You must log in or register to reply here.

Welcome to EDABoard.com

Sponsor

Back
Top