X-Authentication-Warning:	delorie.com: mail set sender to geda-user-bounces using -f
X-Recipient:	geda-user AT delorie DOT com
Date:	Tue, 24 Apr 2012 10:51:31 -0700
From:	Colin D Bennett <colin AT gibibit DOT com>
To:	geda-user AT delorie DOT com
Subject:	Re: [geda-user] They don't call it experience for nothing!!!
Message-ID:	<20120424105131.51db48c8@svelte>
In-Reply-To:	<CALSZ9gpip0jZy6+onHHAJCLufE+Ptq9VCeo3-wLWiH2RcsgdDw@mail.gmail.com>
References:	<CALSZ9gpip0jZy6+onHHAJCLufE+Ptq9VCeo3-wLWiH2RcsgdDw AT mail DOT gmail DOT com>
X-Mailer:	Claws Mail 3.8.0 (GTK+ 2.24.10; x86_64-pc-linux-gnu)
Mime-Version:	1.0
X-AntiAbuse:	This header was added to track abuse, please include it with any abuse report
X-AntiAbuse:	Primary Hostname - gator297.hostgator.com
X-AntiAbuse:	Original Domain - delorie.com
X-AntiAbuse:	Originator/Caller UID/GID - [47 12] / [47 12]
X-AntiAbuse:	Sender Address Domain - gibibit.com
X-BWhitelist:	no
X-Source:
X-Source-Args:
X-Source-Dir:
X-Source-Sender:	spk.venturedesignservices.com (svelte) [65.61.115.34]:55695
X-Source-Auth:	colin AT gibibit DOT com
X-Email-Count:	1
X-Source-Cap:	c2t5bGVuO3NreWxlbjtnYXRvcjI5Ny5ob3N0Z2F0b3IuY29t
X-MIME-Autoconverted:	from quoted-printable to 8bit by delorie.com id q3OIIpHG028167
Reply-To:	geda-user AT delorie DOT com
Errors-To:	nobody AT delorie DOT com
X-Mailing-List:	geda-user AT delorie DOT com
X-Unsubscribes-To:	listserv AT delorie DOT com

On Tue, 24 Apr 2012 13:22:15 -0400
Rob Butts <r DOT butts2 AT gmail DOT com> wrote:

> Who would have thought that pins 1 and 2 are opposite for SOT23
> and SOT23-3?  Too bad PCB didn't have an SC59!
> 
> Well, luckily it is only a 1.5 square inch board!  Although the
> components and a respin are another $50.
> 
> PCB lesson and experience?  Priceless!!!

Ouch, that is a bummer.

What do you mean by "SOT23-3"?

All these references to support the fact that SOT23-3 (3-lead
SOT23, aka TO-236) has pins 1 and 2 together, with pin 3 opposite
them:

[1] "JEDEC TO-236 Solid State Product Outline".
    <http://www.jedec.org/standards-documents/docs/236-h>.
    (free registration required).

[2] "50ppm/°C Max, 50μA in SOT23-3 CMOS VOLTAGE REFERENCE".
    <http://www.xilinx.com/products/boards/ml410/datasheets/ref3025.pdf>

[3] "Low Capacitance Quad Line ESD Protection Diode Arry SM05
    SOT23-3". <http://union-ic.com/upload/13206410863338.pdf>
    See "Pin Configurations" and "Top View" on page 1.

[4] "Littelfuse SP05 Series".
    <http://www.littelfuse.com/data/en/Data_Sheets/Littefuse_TVS_Diode_Array_SPA_SP050.pdf>.
    See "Pinout" for SP0502BAHTG, SP0502BAJTG on page 1.

Is this a pcb footprint library bug or misnaming?  I see that the
'SOT23' footprint has pins 1 and 2 on one edge, then pin 3 on the
opposite edge.  This is the standard 3-lead SOT23 package.

The pcb footprint called 'SOT23D', on the other hand, has pins 2
and 3 on one edge, and pin 1 alone on the opposite edge.  This is a
misleading and flat-out wrong footprint to be called "SOT23".
I think it exists to allow you to use the usual 2-terminal diode
symbol (with pins named "1" and "2") in the schematic, then use
this 3-lead footprint with it.  This is the WRONG way to do it.
The SOT23D footprint should not be used, and you should either

(1) use a symbol that is a specific 3-terminal
    symbol special for the SOT23 diode package (and note pin
    function assignments may vary!), or

(2) use a 2-terminal symbol with _logical_ pin names like "A" and
    "K" with a SOT23 footprint having these logical pin names
    assigned to the physical pins.

Regards,
Colin

- Raw text -