Matthew,
While I am completely unfamiliar with what the UK is doing for specs, I do
have a lot of info available on schematic rules and practices here in the
USA. Some or all of which may be applicable to your desire for some
standardization in the drafting of schematics.
The IPC publishes a document that covers this subject... IPC-D-325.
The copy I have was published in 1995.
Section 10 covers Schematics and Logic Diagrams. Here's a brief synopsis:
Formats should be as small as they can and still comfortably fit the data to
be drawn... where there are multiple sheets all of them should be the same
size...
Abbreviations according to MIL-STD-12
Schematics should be read from left to right, and or top to bottom.
Terminations, connections, etc. should be located on the outer edges of the
drawing...
Connecting lines shall be drawn with as few crossovers and direction changes
as possible, min spacing between lines at 1:1 scale is .25 inches (that's
pretty big actually...)
4 way connection junctions are acceptable but 'not preferred'... (but I say
outlaw them... )
They recommend showing pin numbers for things like resistors and caps where
most of us do not... the rational explanation given says it helps with CAD
data.
It basically mirrors what has been around for years and years that the
industry has used for guidance in creating schematic diagrams...
These specs for drafting schematic diagrams derived from MIL-STD-100 are in
the standard drafting manual published by Global Engineering entitled
"Drawing Requirements Manual" in section 22-4 Electrical and Electronic
schematic diagrams.
It basically says the following:
1) Graphic symbols must comply with ANSI Y32.2/IEEE 315
2) The position of the symbol does not alter its meaning (remember the
ground symbol ?)
3) Symbols may be drawn to any proportionate size or line thickness to suit
reproduction (and thus readability) of the document
4) Electrically operated Symbols shall be shown in the 'power off' or
non-energized state or you will provide a note indicating the otherwise.
5)The terminal symbol (o) may be attached to any wire connection on the
symbol..(I think they are referring to the inversion of the state of a
digital signal as in the case of an inverted input or output on a logic gate
for example...)
6) Symbols that show a relationship between parts - in the case of relays
for example, the separate parts of the relay can be shown on the schematic
in different locations as long as the reference designations tie them
together... i.e. U1-A, U1-B are two parts of a single package and can be
drawing in different sections of the schematic...
7) Switches are shown in a position with no operating force applied
8) Symbols are drawn in a heavier line weight that connecting lines
9) Reference Designations shall comply with IEEE STD 200 (ANSI Y32.16)
10) Complete reference designation - if you had a cap on a board in a unit
that was part of a rack assembly its complete reference designation would
indicate its type of part, and position in its membership to the entire
assembly... for example C4 on your board would really have a complete ref
des of U2-A1-C3 or equivalent. Typically we don't show those complete ref
des on the schematic or the parts list but in a more formal documentation
system that might be required and we are supposed to know that C3 on one
board is not the same as C3 on another board in an electronic assembly
unit... it actually has an address like your home number... it's a unique
location with its 'zip code'... even if there are two streets with the same
name, the post office finds your house don't they... same principle really.
C3 identifies a capacitor on board A4, in housing A1, in rack U6 so the
complete designation is U6A1A4C3. All this stuff is explained in ANSI
Y32.16/IEEE STD 200
11) So... the abbreviated ref des C3 is a 'Partial Reference Designation' by
definition (see above)
12) Reference Designation is NOT and abbreviation for the name of an item.
13) Reference Designations shall be assigned in a consecutive manner
starting with the number 1 and proceed to be assigned in a left to right,
top to bottom sequenced manner.
14) Additional information can be added to the symbols like type
designation, value, watt rating, tolerances, etc... as needed.
15) Numerical values are expressed as whole numbers and decimals.
Use .092uF not 92000pF
Use 5mH not 0.005H
Use 2.5K not 2500 OHMS
16) Don't use the comma in numerical values.
17) Repetition of values should be eliminated through the use of notes:
Unless otherwise specified:
1) Capacitance values are in Microfarads, 10%
2) Resistance Values are in K Ohms, 5%, 1/4 watt
18) Schematics should omit equipment lists... and if used for reference
only, they should not be co-mingled or in the same area as the parts list to
avoid confusion.
Beyond that... the user can use his/her imagination to make the schematic
understandable... notes are good to clarify anything non-standard... and if
there is no standard symbol for your part, use a box with pins going in and
out of it, inputs on the left, outputs on the right...
One other thing I do is give a general direction to power and ground
symbols, power up, ground down... there are exceptions to that based upon
special circuit diagram reading practices, symmetrical circuits might show
the grounds in an upward direction if they have 'counter parts' that are on
the opposite side of a symmetrical RF circuit diagram going down... for
example...
Well that's more than I planned to write, I guess this turned into
Schematics 101... sorry about that.
If you want to dig deeper, there are some 'out of print' books on the
subject that I like... you might find used copies of them from Barnes and
Nobel or Amazon.com...
Electronics Drafting and Printed Circuit Design by James M. Kirkpatrick
Drafting for Electronics by Lamit/LLoyd
Electronics Drafting and Design by Nicholas M. Raskhodoff
The Design and Drafting of Printed Circuits by Darryl Lindsey
Best regards,
Bill Brooks
PCB Design Engineer, C.I.D.+
DATRON World Communications, Inc.
"Performance you require - Value you expect"
http://www.dtwc.com
Tel: (760)597-1500 Ext 3772 Fax: (760)597-1510
-----Original Message-----
From: Matthew Lamkin [mailto:[log in to unmask]]
Sent: Monday, November 19, 2007 3:24 AM
To: [log in to unmask]
Subject: [DC] Current Schematic drawing standards?
Hello, can anyone (preferably from the UK) point to what current schematic
drawing standards there are?
I'm not talking about what symbols should look like as I have EN60617-2 for
that, but more
for how to present a drawing I.E. not to have more than 3 lines into a
junction dot.
Or does a standard not exist for this?
Basically I'm getting completely peed off with the crappy drawings that
engineers are sending me
with what I see as many drawing faults in that are not to what I'd call
standard ways of doing things.
And being engineers they wont conform to damn all unless I can show them a
written standard that
they should conform to.
Grrrr...
Thank you,
Matthew Lamkin.
---------------------------------------------------------------------------------
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
---------------------------------------------------------------------------------
|
