[sdiy] Schematic/PCB layout best practices

Sat Oct 4 08:08:18 CEST 2008

1) I like to do my part numbers based on their sheet location. Assuming 
there are no more than 9 schematics in a set then all the components on 
sheet 1 are 1xx, those on sheet 2 are 2xx and so on. The components are then 
numbered in a general right to left, top to bottom sequence although some 
components will be grouped together to assist with locating them. So, for 
example all the resistors based around a mixer opamp might be numbered R100 
to R107.

Working on the basis that I won't be servicing the pcb everyday, it is a lot 
quicker to look at a board and see R512 is faulty and then jump to sheet 5 
to find what is all about. This approach also makes BOM a breeze to read and 
you can easily sort the parts by sheet. often the sheet forms a specific 
module within the design such as the microcontroller, I/O or comms and this 
just adds to the ease of identifying components on BOM and schematics.

I also find that this numbering scheme makes it easier to lay out boards. 
Generally I have split my schematic in to logical blocks and those blocks 
will generally be grouped together on the pcb. So, in general, all the x2yy 
components will be close together and so will all the x3yy and so on.

If, on the other hand I was a service technician and repairing boards every 
day then there might be an argument for numbering sequential on the pcb.

2) Initially there are 2 track sizes, 15mil for signals and 30mil for power. 
If space permits then increase the power to up to 50mil. In general though 
you will find that one these tracks are near chips, especially, SMD then 
that rule goes out the door. Signals should, ideally, not go below 12mil but 
again certain components and where you need to route through a connectors 
pins you will find a need to drop down. The smallest I have gone to is 7mil 
with an SMD chip.

Another factor is the spacing between adjacent tracks of different nets. 
This spacing, the track thicknesses, the spacing between pins where they 
have to be passed between and the grid you have selected for the track 
routing will determine the best thicknesses.

Try to keep all your power tracks thick to reduce voltage drops. Similarly 
keep your signals as thick as possible. But I think you will find 15mil and 
30mil a good starting point.

Where the design allows, you should have 2 grounds, (1) AGND or analogue 
ground for all your audio signals and general analog circuitry, (2) DGND or 
dirty ground or digital ground for all your digital/logic circuitry. try to 
keep the circuits away from each other trying to minimise the amount of 
digital tracking that needs to go through the analog section. If possible 
divide the board in to analog and digital and keep the circuits within those 
parts. In this case you will also usually have different power rails such 
+5V for the digital and +/-15V for the analogue. You might even have +5V for 
some analog stuff. These should all be generated using separate regulator 
circuits (especially the two 5V rails which should be something like +5VD 
and +5VA for digital and analog) and again kept as far apart as possible.

Don't know about Eagle but you should try to use NET LABELS for as many 
tracks as possible that are important. When working on the pcb the net names 
like AUDIO_OUT will mean a lot more than J101_1....

This forum has had several attempts at discussing grounding of circuits 
including a recent one of grounding to front panels and the controls 
attached.

Try and standardise on your component footprints, 0.4" axials for resistors, 
0.2" radials for capacitors in the range 1nf to 1uF and so on. This will 
allow you to rationalise your stock requirements and with sensible choices 
will make it easier for builders to source themselves. Check all footprints 
to ensure adequate clearance, especially ICs where you will need to allow 
for IC sockets and access to the ends to lever them in and out.

Consider the assembly side when placing components. Put connectors in easy 
to get at places. I don't like having connectors in the middle of a board 
unless necessary. Wiring is much easier and neater if they are around the 
edge of the board. Place trimmers near the edge of boards if practical  and 
use vertical trimmers so that you can get to the trimmer without fighting 
your way through bundles of cables.

Allow a 1mm or more gap around the edge of the board i.e. create a KEEPOUT 
track that runs 1mm inside the edge of the board. This will prevent the risk 
of tracks coming to the edge and getting lost or damaged when the pcb is cut 
to size.
If space permits then run all components the same way, this will greatly 
ease soldering as you will be working in rows and columns.

Best Regards

(Mr) Laurie Biddulph
Phone: +61 (0)2 4340 0938
Mobile: 0400 257 645

Elby Designs
ABN: 70 022 727 605
http://www.elby-designs.com

This e-mail and any files transmitted with it are confidential and intended 
for the addressee only.
If you are not the addressee you may not copy, forward, disclose or 
otherwise use it, or any part of it, in any form whatsoever. If you have 
received this e-mail in error please notify the sender and ensure that all 
copies of this e-mail and any files transmitted with it are deleted.
Any views or opinions represented in this e-mail are solely those of the 
author and do not necessarily represent those of Elby Designs.
Although this e-mail and its attachments have been scanned for the presence 
of computer viruses, Elby Designs will not be liable for any losses as a 
result of any viruses being passed on.

Please consider the environment before printing this email

----- Original Message ----- 
From: "Aaron Lanterman" <lanterma at ece.gatech.edu>
To: "Synth-DIY DIY" <synth-diy at dropmix.xs4all.nl>
Sent: Thursday, December 04, 2008 2:40 PM
Subject: [sdiy] Schematic/PCB layout best practices

> Greeting schematicians and PCBeings,
>
> 1) Is there a Best Practice for numbering components? I'm putting in 
> schematics into Eagles in a semirandom fashion, and am hence getting  them 
> numbered in a semirandom fashion.
>
> I was thinking:
>
> A) It might be best to renumber them based on how they appear on the 
> final PCB, maybe number with increasing numbers left to right or 
> something, to make things easier to find there, or
>
> B) It might be best to number based on the schematic, where say parts 
> near one another in the circuit have similar numbers; or maybe if  there 
> are multiple similar subcircuits, or...
>
> C) Number based on the schematic, but instead have the equivalent  parts 
> in the different subcircuits have similar numbers (i.e. input  resistors 
> R1 through R5, feedback resistors R6 through R10, resistors  to ground R11 
> or R25), or
>
> C) I'm totally overthinking this and should let randomness rule.
>
> 2) What's the Best Practice for choice of trace width for (A) typical 
> signals and (B) power and ground for typical synth module operation? I 
> realize I've been using Eagle's default, which is 0.016 for default,  for 
> signals, and 0.024 for ground and power since it was the next step  bigger 
> from 0.016 from the drop down menu, but then I figured I should  have 
> better reasons for picking values than they happen to be some  Eagle 
> defaults.
>
> 3) Buchla quite often has separate "Quiet" and "Noisy" grounds. He  uses 
> the Noisy grounds in digital circuitry, but he also seems to use  the 
> noisy grounds sometimes in circuitry related to control signals,  in 
> places where it seems hooking things to a "Quiet" grounds would do  no 
> harm. If a circuit I'm working on is pretty much all analog, is the  a 
> compelling reason to keep separate "signal" and "control" grounds,  or can 
> I just lump them all together? Is it related to Buchla using  1/8" for 
> signal but bananas for control?
>
> - Aaron
>
> _______________________________________________
> Synth-diy mailing list
> Synth-diy at dropmix.xs4all.nl
> http://dropmix.xs4all.nl/mailman/listinfo/synth-diy
> 