SPICE models for 1N53nn Zener diodes?

Mike Elliott

unread,

Mar 10, 2003, 7:02:37 PM3/10/03

to

Anyone got a pointer to models for this family of Zener diodes?

MikeE

Jim Thompson

unread,

Mar 10, 2003, 7:14:46 PM3/10/03

to

Couldn't find anything on 1N53xx, that are *zeners*. But here's my
generic zener subcircuit, you can set parameters to suit....

****
.SUBCKT MyZENER 1 2 PARAMS: BV=10 IBV=1m RS=1 IS=10f
D1 1 2 DZ
.MODEL DZ D(
+ IS = {IS}
+ RS = {RS}
+ N = 1
+ EG = 1.11
+ BV = {BV}
+ IBV = {IBV} )
.ENDS MyZENER
****

For proper E-mail replies SWAP "-" and "_"

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

Mike Elliott

unread,

Mar 10, 2003, 8:06:02 PM3/10/03

to

I read that Jim-T@analog_innovations.com said in article
<2eaq6vovlmbsplv4v...@4ax.com>, . . .

> On Tue, 11 Mar 2003 00:02:37 GMT, Mike Elliott
> <j.michae...@REMOVETHEOBVIOUScoxDOT.net> wrote:
>
> >Anyone got a pointer to models for this family of Zener diodes?
> >
> >MikeE
>
> Couldn't find anything on 1N53xx, that are *zeners*. But here's my
> generic zener subcircuit, you can set parameters to suit....
>
> ****
> .SUBCKT MyZENER 1 2 PARAMS: BV=10 IBV=1m RS=1 IS=10f
> D1 1 2 DZ
> .MODEL DZ D(
> + IS = {IS}
> + RS = {RS}
> + N = 1
> + EG = 1.11
> + BV = {BV}
> + IBV = {IBV} )
> .ENDS MyZENER
> ****
>

Thanks, Jim, that's very cool.

Maybe someone can help me with this probably very rudimentary questions
involving usage of Jim's subcircuit with LTspice:

LTspice's diode symbols (zener, etc.) like to use models, not
subcircuits, from the provided standard.dio file.

1. If I have subcircuits for the Zeners I want to use, how can I use
them?

2. If a fellow modifies a file like standard.dio, does he run the risk
of it being overwritten during the next LTspice sync?

MikeE

Jim Thompson

unread,

Mar 10, 2003, 8:27:08 PM3/10/03

to

On Tue, 11 Mar 2003 01:06:02 GMT, Mike Elliott
<j.michae...@REMOVETHEOBVIOUScoxDOT.net> wrote:

I'm sure LTSpice can use subcircuits.

>
>1. If I have subcircuits for the Zeners I want to use, how can I use
>them?

I don't know LTSpice's symbol methods, but you can strip down my
subcircuit to a diode model, but fill in the blanks, e.g.,

.MODEL DZ D(
+ IS = 10f
+ RS = 1

+ N = 1
+ EG = 1.11

+ BV = 10
+ IBV = 1mA )

>
>2. If a fellow modifies a file like standard.dio, does he run the risk
>of it being overwritten during the next LTspice sync?

I know that PSpice updates do overwrite libraries, so I put my
libraries and symbols in a directory of my own. Then, after an
update, I pick and choose what I want to add to my repertoire.

I also back up my .INI and .PRB before an update, then replace what
was put there by the installation.

>
>MikeE

Mike Elliott

unread,

Mar 10, 2003, 8:55:46 PM3/10/03

to

I read that Jim-T@analog_innovations.com said in article

<ufeq6v4pcr9tbkc9q...@4ax.com>, . . .

> >LTspice's diode symbols (zener, etc.) like to use models, not
> >subcircuits, from the provided standard.dio file.
>
> I'm sure LTSpice can use subcircuits.
>
> >
> >1. If I have subcircuits for the Zeners I want to use, how can I use
> >them?
>
> I don't know LTSpice's symbol methods, but you can strip down my
> subcircuit to a diode model, but fill in the blanks, e.g.,
>
> .MODEL DZ D(
> + IS = 10f
> + RS = 1
> + N = 1
> + EG = 1.11
> + BV = 10
> + IBV = 1mA )
>
> >
> >2. If a fellow modifies a file like standard.dio, does he run the risk
> >of it being overwritten during the next LTspice sync?
>
> I know that PSpice updates do overwrite libraries, so I put my
> libraries and symbols in a directory of my own. Then, after an
> update, I pick and choose what I want to add to my repertoire.
>

Thanks, Jim. I can see how to distill a .model out of the .subcircuits.

LTspice's zener model syntax is:

.model DIODENAME D(Is=1.5n Rs=.5 Cjo=185p nbv=3 bv=6.2 Vpk=6.2
+ mfg=Motorola type=zener ) -- close enough.

It would be easy-peasy to add the models to LTspice's "standard.dio"
file, but that does leave the worry that LTspice will overwrite it at
the next release sync. So I should create my new models in "my.dio"
file.

I'll post the following question to Mike Englehardt: how can I get the
schematic's Diode symbol inserting thingy to read the "my.dio" file?

MikeE

Mike Elliott

unread,

Mar 10, 2003, 9:10:19 PM3/10/03

to

I read that j.michae...@REMOVETHEOBVIOUScoxDOT.net said in article
<MPG.18d6e1e69...@news.west.cox.net>, . . .

> I read that Jim-T@analog_innovations.com said in article
> <ufeq6v4pcr9tbkc9q...@4ax.com>, . . .

Wait - never mind. LTspice's Help answers the questions:

"For example, 1N5234 has a zener voltage of 6.2V. The simplest model is
as follows: .model 1N5234 D(BV=6.2)

Use the [File] [Open] command to open the diode database:
.\lib\cmp\standard.dio and insert the desired models, if necessary The
[Sync Release] will preserve the user's models as long as the model
names are different from the default models provided by LTC."

MikeE

Jim Thompson

unread,

Mar 10, 2003, 9:18:51 PM3/10/03

to

On Tue, 11 Mar 2003 02:10:19 GMT, Mike Elliott
<j.michae...@REMOVETHEOBVIOUScoxDOT.net> wrote:

>I read that j.michae...@REMOVETHEOBVIOUScoxDOT.net said in article
><MPG.18d6e1e69...@news.west.cox.net>, . . .
>> I read that Jim-T@analog_innovations.com said in article
>> <ufeq6v4pcr9tbkc9q...@4ax.com>, . . .
>
>Wait - never mind. LTspice's Help answers the questions:
>
>"For example, 1N5234 has a zener voltage of 6.2V. The simplest model is
>as follows: .model 1N5234 D(BV=6.2)
>
>Use the [File] [Open] command to open the diode database:
>.\lib\cmp\standard.dio and insert the desired models, if necessary The
>[Sync Release] will preserve the user's models as long as the model
>names are different from the default models provided by LTC."
>
>MikeE
>
>> >

[snip]

You'll probably want to set "IBV", the current at which "BV" occurs,
and probably the series resistance, "RS", as well.