subject: pcb design techniques (long)
from: leon heller (leon_heller@hotmail.com)
date: mon oct 07 2002 - 10
50 edt
next message: leon heller: "re: how old are we?"
previous message: rob matherly: "re: age, years licensed"
--------------------------------------------------------------------------------
i few weeks ago i posted some notes on making pcbs, which received a
favourable reception. here are some notes in a similar vein, about the
process of designing a single-sided pcb for making at home. they are
basically 'rules of thumb'. btw, do you know the origin of this term? in
the good old days, when wife-beating was a popular pastime, it was
decreed that the stick employed should be no thicker than a man's thumb.
i'll assume that you have some sort of suitable cad system, although the
techniques should be applicable to the classic technique of designing
the layout on squared paper, using a pencil, and lots of rubbing out. a
college friend of mine many years ago was very good at engineering
drawing, and usually finished an hour before everyone else. to relieve
the tedium, he indulged in what he called 'negative drawing', rubbing
out what he had done and redrawing it. 8-)
you start with a schematic, of course. most packages have schematic
capture integrated with pcb layout, so that you go from a schematic to a
'rats nest' of components and 'rubber-banded' interconnections or
'air-wires'.
i use conservative design rules for many of my home-made pcbs - 15/15
for signal tracks and 25 or 50 mils for supply tracks. by 15/15 i mean
15 mil wide tracks with a minimum separation of 15 mils. i can go down
to 12/12 if necessary. most pads (ics for instance) have 0.8 mm holes
(about .030"). with the pad size i use on ics, 0.8 mm doesn't leave much
'meat' around the hole, so i've started to use a 0.7 mm drill on these
holes. in europe we tend to use a mixture of imperial and metric when
designing pcbs. it can get a bit confusing. we usually refer to a 'mil'
as a 'thou', btw.
most packages will check for design rule violations - tracks too close
to pads, tracks too close to each other, etc. mine can, optionally, do
this in real-time, but i find it distracting.
component placement is all-important, and it is worth spending a lot of
time on it. get it right, and it makes the routing very much easier.
some cad packages will place the components for you, minimising the
track lengths, but the board will look a real mess, and will be very
difficult to route.
i find that it's generally best to follow the schematic, and group
associated components together.
if you have constraints on the board size, place the correctly
dimensioned board outline at this stage. i usually just put in a large
outline, lay the circuit out, and then adjust the outline to suit it.
position connectors and controls along the edges of the board. usually
the controls will be at the front and the connections at the back. make
sure all the connectors are oriented the same way, and try to minimise
the track lengths to the circuitry they connect to, especially if they
are carrying signals. this applies to the controls, also.
now start positioning the ics and other large components. again, orient
them the same way. this might make the routing harder, but the results
look much neater. the ics should be lined up so that all the ends (pin
1) are in line, and space them an equal distance apart. position the ics
etc. so that you minimise the amount of track crossings, and track
lengths.
now you can start adding the passive and discrete components. start with
the important ones like decoupling capacitors, and get them nice and
close to the positive supply pins. then position the remaining passives.
if you have several resistors, arrange them above one another, instead
of staggering them, and use the same spacing between them. move other
components if necessary, to get them all in.
when you are happy with the layout, you can start routing the board,
laying down the tracks. whilst autorouters can work quite well on
multi-layer digital boards, most of them cannot cope with single-sided
boards, and boards with lots of analogue stuff.
put in the power supply tracks first - vcc and ground, as a rule. try to
have nice fat tracks with connections to the power pins and decoupling
capacacitors coming off as spurs, rather than just daisy-chaining them.
it's a good idea to adopt a gridded layout, if you have more than a few
chips.
the package i use has a very useful copper pour facility. i just route
the vcc connections, route the other connections, and finally, use the
copper pour to connect all the ground pins. i often have to put in a few
redundant links, and move things around a bit, to get all the grounds
connected, but it saves a lot of time, looks nice, and provides a good
low-impedance ground return. it also minimises the amount of etchant
used. i use the hatched option, as laser printers aren't usually very
good with large black areas. my software also puts in thermal reliefs
(spokes from the pad to the surrounding copper) to make soldering
easier.
having sorted out the power connections, you can now start on the signal
tracks. it's usually best to route the shortest ones first, moving
components around as required. i can get a single 15 mil track between
0.1" spaced ic pins, with a 55 mil diameter pad, observing the 15/15
design rules. it's a good idea to periodically check for design rule
violations, and correct them as you go along, than to finish the thing,
and find that you've got dozens of errors.
sometimes you will need to add a wire link on the top of the board. i
use my software in double-sided mode, so that the links are,
effectively, connections on the top layer. this ensures that checking
against the original schematic works properly. even if you can route a
track all over the place on the bottom side, it's often a good idea to
simply insert a link. it minimises the board size, and could help with
nasties like crosstalk.
once i've got the board routed, and it passes the design rule checks,
and it still matches the schematic, i generate a net completion report.
for instance, this tells me whether i've got any 'split nets', such as
ground connections in one part of the board that aren't connected to the
ground pins in another area. this is usually due to the copper pour
being unable to reach all the ground pins, and i simply juggle things
around, insert links, and so on, until i get complete connectivity.
that's basically it. if you want to play with pulsonix, the software i
use, you can download an evaluation copy (a rather large file) from:
http://www.pulsonix.com when using it for your own designs, it's restricted to not more than 100
pins, but you might still find it useful. if anyone gets it, and wants
one or two of my simpler designs to play with, i can email something
that illustrates the techniques i use.
73, leon
--
leon heller, g1hsm
leon_heller@hotmail.comhttp://www.geocities.com/leon_heller
