SOT23 pin numbering

[Joerg]

What is the current convention with respect to pin numbers on SOT23?

I have seen:

Zetex 1
=====
3 2

Then OnSemi 3
=====
1 2

And Infineon (also in an older Siemens data book)

3
=====
2 1

Somehow that looks like an invitation to a huge mess. What gives? Which
one is now "standard"?

Regards, Joerg

 

[Brad Velander]

Joerg,
Yeah you are right, I don't know that there is one and only
one standard in theory but there certainly isn't in practice.
Typically what I and others I know do is decide on one company
standard for SOT23 pin numbering and then stick to it. You may
even cover it in a note on your assembly drawings and schematics
so that there is no confusion down the road when someone sees a
schematic symbol that doesn't match the manufacturer's pin
numbering.

FYI, I standardize on:
3
====
1 2

In my experience that one covers 80 - 90% of the
manufacturer's devices I have ever used.

That said, my present employer standardized long before I
arrived on:
1
====
2 3

 

[Paul Burke]

What is the current convention with respect to pin numbers on SOT23?

Why number at all? Name them ebc, gsd or whatever, and hide the numbers
on the schematic. If it's going to be critical for the techies, print
the names on the silkscreen or on a diagram in a maintenance document.

They seem to be pretty standard in SOT23- have I missed the odd men out?
And why did we end up with such a mess with TO92s, where even the same
numbered part can have variant pinouts?

Paul Burke

 

[Joerg]

Hello Brad,

Yeah you are right, I don't know that there is one and only
one standard in theory but there certainly isn't in practice.
Typically what I and others I know do is decide on one company
standard for SOT23 pin numbering and then stick to it. You may
even cover it in a note on your assembly drawings and schematics
so that there is no confusion down the road when someone sees a
schematic symbol that doesn't match the manufacturer's pin
numbering.

FYI, I standardize on:
3
====
1 2

In my experience that one covers 80 - 90% of the
manufacturer's devices I have ever used.

Same here, but the picture changes for European parts. I wonder what IPC
and all this bureaucracy is good for when their can't even push through
a standard for the pinout of a simple transistor case.

Regards, Joerg

 

[Joerg]

Hello Paul,

Why number at all? Name them ebc, gsd or whatever, and hide the numbers
on the schematic. If it's going to be critical for the techies, print
the names on the silkscreen or on a diagram in a maintenance document.

That is ok if you do your own layout. But send it off like is customary
and the CAD system of the layouter will pick whatever is its SOT23
variant. Worst case you have a major disaster when the board comes back.
That is one reason why I am hesitant to base this data exchange on
netlists. If the layouter doesn't use the same CAD he or she usually has
to re-generate the whole schematic. Sad, but it prevents pin-out disasters.

Regards, Joerg

 

[Joel Kolstad]

Why number at all? Name them ebc, gsd or whatever, and hide the numbers
on the schematic.

The problem is that you then have to make a new footprint for every new
schematic part -- something most people would prefer to avoid in the name of
saving time!

 

[Joerg]

Hello Joel,

The problem is that you then have to make a new footprint for every new
schematic part -- something most people would prefer to avoid in the name of
saving time!

Right now it is worse. Every good layouter will pull all the data books
to see where what is. Else you'd receive a board, plug it in and
kabloom. "Oh, but in my CAD package the top is pin 1...."

Regards, Joerg

 

[Ken Smith]

The problem is that you then have to make a new footprint for every new
schematic part -- something most people would prefer to avoid in the name of
saving time!

You don't have to do that. You just have to make a new footprint every
time there is a different arrangement of pins.


E E B B C C
B C C B E C C E B E E B

There are only six to make for the bipolars and then you can stop having
to manually edit net-lists. If you have to lay out 6 PCBs with NPNs in
them, there is sure to be a time savings.

 

[Brad Velander]

Joerg,
If your PCB Designer has to re-enter anything then they are
responsible for ensuring their version matches yours. So that is
not really a valid concern. Like I said, a simple note in the
schematic would suitably put them on notice as to your numbering
convention. If they re-enter the works then they can use any
convention that they want but it is their responsibility to match
your overall netlist.
Using the EBC, GSD, etc. is also fine but myself I hate that
system. Can't say why other than some CAD systems don't support
it or don't support it nicely. It also means that you do have to
maintain a number of identical (physically) footprints. There
again is one of my pet peeves, my current employer requires each
company part number to have a unique footprint identified by the
company part number. What a maintenance nightmare (should I call
it an opportunity? Or maybe job insurance, since there is always
library maintenance to do?).

 

[Brad Velander]

Joerg,
I also found that the parts specific to the RF and microwave
worlds varied a lot more than the general jelly-bean variety
transistors.

I don't think you can blame the IPC, maybe Jedec or IEEE (and
other packaging standards) but not the IPC. As far as I have ever
seen, the IPC doesn't spec packages. Only how to deal with them
in PCB design and assembly.

 

[James]

You don't have to do that. You just have to make a new footprint every

time there is a different arrangement of pins.


E E B B C C
B C C B E C C E B E E B

There are only six to make for the bipolars and then you can stop having
to manually edit net-lists. If you have to lay out 6 PCBs with NPNs in
them, there is sure to be a time savings.

In some CAD packages you don't even need to do that, you just need one
schematic symbol with any pin order, one footprint symbol with any pin order
then each part has references to the schematic, footprint and a table of
what pins in the schematic symbol tie up with which pins in the footprint
symbol just for that particular part.

 

[Joerg]

Hello Brad,

If your PCB Designer has to re-enter anything then they are
responsible for ensuring their version matches yours. So that is
not really a valid concern. ...

That's not quite how I see it. My clients are the main concern. They are
my clients as well as the layouter's clients. So together we have to
make sure that things pan out nicely. A blame game later helps nobody.

....Like I said, a simple note in the
schematic would suitably put them on notice as to your numbering
convention. If they re-enter the works then they can use any
convention that they want but it is their responsibility to match
your overall netlist.

Which brings up the point that you have to re-generate all the library
parts or at least check them one by one. I am using Eagle but it was
similar in others: You can find SOT23 and other packages with various
pin numbering schemes among library files.

Using the EBC, GSD, etc. is also fine but myself I hate that
system. Can't say why other than some CAD systems don't support
it or don't support it nicely. It also means that you do have to
maintain a number of identical (physically) footprints. There
again is one of my pet peeves, my current employer requires each
company part number to have a unique footprint identified by the
company part number. What a maintenance nightmare (should I call
it an opportunity? Or maybe job insurance, since there is always
library maintenance to do?).

CAD systems usually do not support EBC. They support 123. Or sometimes
321. The next day you pick another part and it may be 312. So I
understand your employer very well. They want to avoid a major pitfall.
In some more heavily regulated environments it goes further. Being that
specific is law there.

Regards, Joerg

 

[Joerg]

Hello Brad,

I also found that the parts specific to the RF and microwave
worlds varied a lot more than the general jelly-bean variety
transistors.

The topper was when I found that the pin numbers on the SOT package of
the same (!) device changed from a Siemens data book to the Infineon
spec. Yet Infineon is the former Siemens semiconductor branch. That blew
my mind.

It was for the BAV99, pins 1 and 2 reversed. When you accidentally swap
pins 1 and 2 because of such a mess and use lots of BAV99 as VCC/GND
input clamps this will result in an impressive plume of smoke upon
power-up. A meter usually won't show a short because of the two diode drops.

I don't think you can blame the IPC, maybe Jedec or IEEE (and
other packaging standards) but not the IPC. As far as I have ever
seen, the IPC doesn't spec packages. Only how to deal with them
in PCB design and assembly.

I don't want to blame anyone. But I do expect standard bodies to work
together and not do the "oh, it's not our turf" thing. In the same way
that my clients expect me to work together with whomever is their layouter.

Regards, Joerg

 

[Joerg]

Hello James,

In some CAD packages you don't even need to do that, you just need one
schematic symbol with any pin order, one footprint symbol with any pin order
then each part has references to the schematic, footprint and a table of
what pins in the schematic symbol tie up with which pins in the footprint
symbol just for that particular part.

Well, yes, that's how mine does it (Eagle). But when you send off to the
layouters and they use another then you can only hope that they
carefully read the notes since their CAD might assume another pin order
on the package (footprint symbol).

Regards, Joerg

 

[Paul Burke]

In some CAD packages you don't even need to do that, you just need one
schematic symbol with any pin order, one footprint symbol with any pin order
then each part has references to the schematic, footprint and a table of
what pins in the schematic symbol tie up with which pins in the footprint
symbol just for that particular part.

That's what I meant. I sort of assumed tbat all PCB CADs were as
rational as EasyPC.

Now if only they'd put in proper back annotation and hierarchical
schematics...


Paul Burke

 

[Brad Velander]

Joerg,
Ok, saying it was not a concern may have been less than an
ideal way to word it. But when you consider that they 'may' edit
anything that you gave them because of particular issues with
their CAD system or the manner in which they prefer to work, it
becomes their responsibility by default.

Your comment about libraries brings me to one point that I am
adamant about, don't trust canned libraries. At best use them as
a starting point but thoroughly check every part that you take
from them. I suggest taking those parts out to a separate library
such that you can remain very clear on which parts have been
checked thoroughly.

Usually by the time the parts have been properly checked, you
could have made them from scratch just as quickly. If you don't
believe me just consider what you must do to thoroughly check
them? What do you need to do when creating them from scratch? Not
much difference is there? The actual creation/drawing/placing
time is far less than the detailed measures and calculating the
land pattern geometry.

 

[Paul Burke]

don't trust canned libraries.

Amen, amen, amen and amen. Especially Easy PC's, which shows all the
symptoms of having been made by an unsupervised bored student on an
ill-paid summer job.

Usually by the time the parts have been properly checked, you
could have made them from scratch just as quickly.

Especially if you take into account the need for different footprints
for different manufacturing technologies etc.

Paul Burke

 

[Joerg]

Hello Paul,

That's what I meant. I sort of assumed tbat all PCB CADs were as
rational as EasyPC.

Eagle is that rational, too. I really like it although the generation of
new library parts is not nearly as easy and intuitive as it was in OrCad.

Now if only they'd put in proper back annotation and hierarchical
schematics...

Back annotation, yes, but hierarchical schematics is one of the serious
shortcomings of Eagle. OrCad had that from the beginning.

Regards, Joerg

 

[James]

That's what I meant. I sort of assumed tbat all PCB CADs were as rational

as EasyPC.

You assumed that all PCB CAD packages were as rational as EasyPC. I've
previously used a high-end Mentor Graphics package - retailing for £50k
PCB/£25k Schematic - that is not as rational and where you did have to
create every combination (or would it be permutation?) of schematic/pcb pin
number mapping. I suspect by the way the way library kept growing that the
powers-that-were, controlling the standard company library, decided to
create new symbols and footprints for every new part - what a waste!

Now if only they'd put in proper back annotation and hierarchical
schematics...

At present I mainly use Pulsonix which is EasyPC's bigger cousin and has
proper back annotation and hierarchical design. I guess WestDev/NumberOne
Systems want to keep the two products separate because of their different
markets and prices.

James

 

[James]

Well, yes, that's how mine does it (Eagle). But when you send off to the

layouters and they use another then you can only hope that they carefully
read the notes since their CAD might assume another pin order on the
package (footprint symbol).

Ah! I didn't realise you were using different schematic and layout tools.
I've never been in that position myself but I see where your coming from
now.

James