At 03:57 PM 9/5/01 -0700, Brad Velander wrote:
>         If you receive information as a netlist only, then the customer is
>responsible anyways right? They have to have used the right symbol with the
>right part. If they didn't how can you possibly tell?

Ah, but the client is always right unless it can be proven otherwise. I've 
had this very problem (confusion over pin assignments on SOT-23 parts or on 
diodes or on polarized capacitors). Since there is no universal standard, 
it is *my* error if I assume that the customer has matched what is in my 
footprint library. So I have to translate the pins, and it is much easier 
to understand 1 = E, 2 = B, 3 = C, for example, than a purely numerical 
jumbling. (And I have and still occasionally use, a program that makes net 
list changes, including pin substitutions, from a text file. When I use 
this tool, I provide the correction file to the client and ask him to 
verify all such changes.)

Further, even when I can -- to my own satisfaction, at least -- prove that 
the error was the client's, the client may tend to consider me responsible. 
I've certainly lost clients over disputes like this, so if I am to continue 
to earn my reputation as a design professional, I need to do whatever I can 
to lessen the possibility of error.

Technically, since I submit placements -- which obviously include 
footprints and also the net assignments of pins -- and the completed design 
to the client, and the client engineer has approved it, *every* error that 
goes to fab is the client's responsibility. My legal responsibility for 
errors extends only to making good what I provide to the client; with a 
SOT-23 error, that is normally a few minute's work. But for the client it 
can be a disaster.

>         Also, I don't display the pin numbers on transistors or diodes. As
>you said it would convey no more clarity because of the mixture of
>manufacturer numbering/labeling schemes. Likewise the EBC and GDS conveys no
>more information either (without the datasheet). Right? Stalemate!

No, not right, and therefore not stalemate? (i.e., not six of one and a 
half dozen of the other.)

Pin numbers in a net list convey *nothing* about the pin assignments, 
neither as they were on the schematic, nor as they are on the footprint. 
Since there is no standard for either of these assignment sets, to complete 
and to check a design one must refer to three sources: the mfr data sheet, 
the schematic itself (or at least the symbol), and the footprint. If there 
is any mismatch between the three sources, there will be an error.

To a designer working from a net list, the net list takes the place of the 
schematic. There is no way to verify that a net list with numbers is 
correct merely by using the data sheet, the net list, and the footprint, 
because one arbitrary assignment is missing. If one has used appropriate 
letter names, the net list fully replaces the schematic. One need only look 
at the mfr data sheet and the footprint to verify that pins have been 
correctly assigned.

It is always necessary to verify -- if one is to be thorough -- that a 
footprint matches the physical part; further, a part which is logically the 
same may have a differing footprint; so the checker will take the complete 
part number -- which might well be in the net list in the comment field but 
in any case is necessary for design --, look it up, and assign a footprint 
to it. This footprint will always be correct for that physical part, what 
is used on the schematic symbol is practically irrelevant. If the client 
has used numbers on the schematic, Protel's netlist load process will flag 
a mismatch error, forcing me to make a translation. Making that 
translation, obviously, I will need to check the mfr data sheet as well as 
the schematic. From a printed schematic with the numbers suppressed, there 
is no way for me to determine the number assignments (Protel Schematic does 
not allow inspection of this without going to the library, a fairly serious 
shortcoming) except by inferring them from what else is in the net.)

I'll say this: I've convinced myself, rather completely, that functional 
pin names, i.e., letters, should *always* be used for parts like diodes and 
transistors. I have not always done this, especially where I brought 
libraries in from Tango which had been used with clients using older OrCAD 

We have a library committee, and I will so argue on the committee list. The 
plan, as I conceive it, involves a cross-reference between mfr. part number 
and Protel footprints (and perhaps symbols as well). The footprint library 
can be unconditionally correct if letters are used; otherwise, with 
numbers, we would need to decide on a standard assignment *and* verify that 
we have followed that assignment.

Working alone, where one person has control of the schematic and pcb 
libraries, if one wants to use numbers, it would not be such a problem. 
Except that we forget that each day, in some sense, we are a different 
person. Certainly I don't know now what I thought was right five years ago, 
in many cases. Further, if I want to be able to use parts from others, 
these parts should meet some standard, otherwise I'll have to check each 
one in detail (and thus one of the major time-savers in having a shared 
validated library will be lost).

One of the strongest proofs, to me, is that I have seen many errors end up 
in fab due to the use of numbers for pins. Some of these errors would have 
been avoided by the use of functional letters. The remaining errors were 
due to an assumption that one part, similar to another, had the same 
footprint. This error would occur in any case (i.e., it is an error in 
footprint assignment itself).

Abdulrahman Lomax
Easthampton, Massachusetts USA

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
* To leave this list visit:
* Contact the list manager:
* Forum Guidelines Rules:
* Browse or Search previous postings:
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Reply via email to