I've always 'standardized' on using pin 1 for cathode as well.
But the 'crux of the biscuit', I think, lies more in the situation.
If you are part of an in-house scm-pcb design service it should be pretty
easy to dictate a standard ie. cathode=pin1 or cathode=CATHODE. Do it or
you're fired! :)
If you work in a service bureau however, with various customers, this is
utterly impossible to implement. I've seen every possible combination by
now, even mixed numeric and alpha in the same part!
#1 Rule of a pcb designer: trust no one.
Every design I receive, before footprint assignment, is scanned manually
for 2,3,4pin parts to verify the pin#s will match to the footprint pin#(or
name). And this doesn't just apply to diodes or transistors (although
usually the easiet culprit) but also to switches, pol.caps, special
connectors, ect.
My other rule is to change the customer scm as little as possible (less
chance of me creating an error) and create an alternate footprint,
renumbered to match the scm pinout. So I might have several SOTs ie.
SOT23-123, SOT23-231, ect. It's not a perfect solution, but one that has
kept me more sane over the years.
Every engineer is different out there in how they design: some are very
attentive to every detail; some just want to crank out the design as
quickly as possible and don't know (or don't care) if diodes have different
pin labels (especially if they aren't visible). And often parts of circuits
are copied from other, older designs, complicating the issue further.
So, from a service bureau standpoint, I can't see how a standard on
component pinout could ever be a reality -unfortunately.
Just my 2c worth -ymmv.
Ron O
At 12:36 PM 20/03/07, you wrote:
>I think this discussion illustrates why standardization is so important.
>
>For a moment, put yourself in the shoes of the assembly house... If each one
>of you designers were sending your boards to the same assembly house with
>your 'standard pin one assignments'... The assemblers could be very confused
>trying to interpret the differing methods used in your data.
>
>Not only that, but I imagine each of you as experienced designers has a
>different method of graphically indicating the polarity of the parts on your
>boards. Some use a dot, or a fat line, a plus or minus symbol, a schematic
>symbol drawn in the legend, the numeral one, a small triangle or square, a
>pad shaped differently than the others in the part, etc.
>
>While this may seem trivial to some from the designer's perspective, it can
>cause a great deal of trouble for the folks who are using your database to
>build from. Imagine trying to keep track of and interpret each person's
>methods... One customer does it their way, another does it a different way
>and still another has some other way of doing it.
>
>In my case, for example, the Altium Designer program I use gives the
>designer the option of not calling the pin out with a 'number' but allows
>using alphanumeric representation for the pins... so I can call the Anode
>'ANODE' and the Cathode 'CATHODE'... there are no numbers needed in the
>database or netlist for that particular footprint. This works just as well.
>
>Obviously, not all CAD programs let you do that...
>
>In the past when I have used programs that restrict you to the use of a
>number, the Cathode has always been the 'polarized' end with the polarized
>mark on the body. The 'standard' I have always used is to put pin one on the
>polarized end of the part. In the case of the diode, that would be the
>cathode end. That is true of capacitors, as well. The polarized pad would
>typically be called 'pin 1'.
>
>This practice goes way back to the early 1970's when I first started doing
>board design. The Bishop graphics book, published back in the early 1980's
>emphasized the importance of indicating the polarity of components and when
>we moved to CAD in the early 1980's the pin one for the cad footprint and
>schematic symbol was always on the polarized end of the part.
>
>
>Good discussion... :)
>
>
>Best regards,
>
>Bill Brooks
>PCB Design Engineer, C.I.D.+
>Tel: (760)597-1500 Fax: (760)597-1510
>Datron World Communications, Inc.
>Vista, California
>
>
>-----Original Message-----
>From: Kevin L. Seaman [mailto:[log in to unmask]]
>Sent: Tuesday, March 20, 2007 6:14 AM
>To: [log in to unmask]
>Subject: Re: [DC] Footprint standards for Polarized components (Diodes)
>
>Gary,
>
>We use CAD tools that allow alphabetic pin "numbers".
>
>So, we use A and C as pin "numbers" for both the schematic symbol
>and the PCB footprint of all diodes.
>
>For SOT23 diodes we use AA, AC, CC, and NC as required.
>
>For transistors, we use E, B, C, G, S, and D.
>
>This has eliminated all polarity problems with these parts.
>
>Thank you,
>
>Kevin L. Seaman
>OrCAD CIS & Allegro PCB Library Liaison
>Sr. Staff PCB Layout Engineer
>Broadcom Corp. Irvine, CA
>(949) 926-5656
>
>========================= Original Message ==========================
>
>From: DesignerCouncil [mailto:[log in to unmask]] On Behalf Of Gary
>Bremer
>Sent: Monday, March 19, 2007 6:25 PM
>To: [log in to unmask]
>Subject: [DC] Footprint standards for Polarized components (Diodes)
>
>Hi,
>I have been asked if there is a standard for creation of footprints
>espicially for diodes. One of the designers reversed the cathode and anode
>causing all the diodes to be placed backwards. The rational was the pin 1
>was the anode for this device for other diodes pin 1 is the cathode.
>
>Gary Bremer CID
>Manufacturing Engineer
>
>_________________________________________________________________
>Exercise your brain! Try Flexicon.
>http://games.msn.com/en/flexicon/default.htm?icid=flexicon_hmemailtaglinemar
>ch07
>
>---------------------------------------------------------------------------------
>DesignerCouncil Mail List provided as a free service by IPC using LISTSERV
>1.8d
>To unsubscribe, send a message to [log in to unmask] with following text in
>the BODY (NOT the subject field): SIGNOFF DesignerCouncil.
>To temporarily stop/(restart) delivery of DesignerCouncil send: SET
>DesignerCouncil NOMAIL/(MAIL)
>Search previous postings at: www.ipc.org > On-Line Resources & Databases >
>E-mail Archives
>Please visit IPC web site http://www.ipc.org/contentpage.asp?Pageid=4.3.16
>for additional information, or contact Keach Sasamori at [log in to unmask] or
>847-615-7100 ext.2815
>---------------------------------------------------------------------------------
>
---------------------------------------------------------------------------------
DesignerCouncil Mail List provided as a free service by IPC using LISTSERV 1.8d
To unsubscribe, send a message to [log in to unmask] with following text in
the BODY (NOT the subject field): SIGNOFF DesignerCouncil.
To temporarily stop/(restart) delivery of DesignerCouncil send: SET DesignerCouncil NOMAIL/(MAIL)
Search previous postings at: www.ipc.org > On-Line Resources & Databases > E-mail Archives
Please visit IPC web site http://www.ipc.org/contentpage.asp?Pageid=4.3.16 for additional information, or contact Keach Sasamori at [log in to unmask] or 847-615-7100 ext.2815
---------------------------------------------------------------------------------
|
