Kim Lester wrote:
> Brian And everyone,
> I was just about to post a very similar message.
> I'm currently very irritated because I just found a library problem
>  Gripe 1: There are no matching (default) PCB footprints 
>    for the schematic symbols.

  What would you have the default be? (Through-hole or SMT?)

>  Gripe 2: The schematic symbol for a pot has pin 3 as the tap/wiper.

  ALWAYS, ALWAYS, ALWAYS check pins found on schematic library parts to
those YOU are going to use and verify the PCB library footprint is
appropriate. (whether it is a 2 pin diode or capacitor or a 560pin

>  Question:  What is the correct way of assiging schematic pins ...
>  Question: Do I have to create my own compatible sch and PCB libs ...

If I had the power, I would insist that Protel (and ALL other EDA
vendors) put a notice on the opening screen for (first time) users:

  Use the enclosed libraries at your own risk!
  1) Review ALL components chosen from the library to make sure
      it is correct for your application, component vendor, board
      fabrication facility, assembly shop, customer and consumer.
  2) Check EVERY pin of the device. Check for unused pins (e.g. No 
      Connect), check for correct power and ground pins (I/O 
      vs CORE), UNHIDE ALL pins for use on schematics, ADD any
      missing pins that are not used for any purpose whatsoever
      (they will be required in the next lot of material received
      from the IC vendor!!).
  3) Copy the validated device to a NEW library (e.g. MYLIB.lib) 
      so future upgrades to the software do not overwrite all of
      your verification efforts. ONLY USE THE NEW library (i.e.
      MYLIB.lib) for insertion of components into schematics (or
      PCB designs as the case may be). 
  4) Make sure the schematic pin names match the footprint pin names
  5) When validating a footprint, check with the assembly shop to
      make sure of their requirements regarding:
        a) solder stealing pads,
        b) changes of footprint relative to placement orientation
        c) pin out from (this week's) IC vendor
        d) placement (and size, clearances) of fiducials
        e) usage of a footprint for an obsolete device

I do not know how many times new (and not so new) users of a particular
package have grabbed a component from one of the libraries and then
found out that there is a problem on the board they are debugging. When
I get libraries from clients that have "verified" components, I recheck
them as I have found problems in the past.

 One of my clients commonly uses two SMT LEDs that use the same
footprint (one of the SMT pads is larger than the other, but there is no
marking on the device); however, the anode and cathodes are reversed
between the devices. I usually get a schematic (or netlist) specifying
"LED", and when I try to get clarification, it is usually something like
"just use the ones on the boards Joe built." I envy those of you who
have clients that specify part numbers (in house or vendor). 
 I have even found footprints for both parts present in a single netlist
from this customer! (This is REALLY nice for the assembly shop since the
BOM generally just would say LED!)

 With many designs making use of "reuse" I have found clients designs
that copied pages from previous designs, just to find out components
were now obsolete! (Guess who gets blamed if the obsolete part footprint
gets placed on the board!)

  (For those of you who actually read this far, I know there *may* be
some situations that seem to warrant the use of hidden pins; however, I
can no longer justify their use even for the simplest of designs.)

David W. Gulley
Destiny Designs

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
*  This message sent by: PROTEL EDA USERS MAILING LIST
*  Use the "reply" command in your email program to
*  respond to this message.
*  To unsubscribe from this mailing list use the form at
*  the Association web site. You will need to give the same
*  email address you originally used to subscribe (do not
*  give an alias unless it was used to subscribe).
*  Visit
*  to unsubscribe or to subscribe a new email address.
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *


To leave the EDAFORUM discussion list, send a email with
'leave edaforum' in the body to '[EMAIL PROTECTED]'

More Information :

Reply via email to