[Diy_efi] circuit and PCB proofreaders?
Tue Apr 11 12:44:35 UTC 2006
----- Original Message -----
From: "Steve Ravet" <Steve.Ravet at arm.com>
Subject: [Diy_efi] circuit and PCB proofreaders?
Before I send it off I'd appreciate some comments, especially on the PCB and
any issues that may affect reliability or manufacturability.thanks
Nice schematic! I like the way you partitioned up the PIC symbol, I'll have
to try that myself the next time I create a schematic.
On the PCB layout, I have a few tips I can recommend, I'll list them here
(in no particular order).
1) You seem to have used minimal width tracks throughout the PCB. Why not
consider making them thicker; you could probably get at least twice as thick
and still be able to cleanly get into those surface mount pads on U2.
2) Try making the pad that you use for the vias a bit bigger. That way, if
the drill is not quite centered, you wont run the risk of creating an open
circuit between the via and the track.
3) Try and pour copper on both sides of your board and connect it to your
ground signal. This will have the benefits of greatly improving your EMI /
EMC performance whilst reducing the amount of waste copper that your PCB
manufacturer has to throw away.
4) I would consider moving U1 closer to the USB connector. There will be
some high frequency signals on the USB lines and I'd try and kep it away
from other signals if possible.
5) Be careful when positioning the tracks to your crystal oscillator. As a
rule, you should never run any other signals in between the tracks tyo your
crystal. Try to place the crystal as close as possible to the micro to
reduce the track length. For example, a better position for Q2 would have
been on the left side of U1, with the tracks being as direct as possible.
6) The decoupling caps that you have on your board need to be as close as
faesibly possible to the ICs. In their current position, they will be of
little use, especially with the thin tracks. Try to keep them within 10mm
of the power pins of the IC.
7) I would have a look at the design rules you have set up for this board.
There are some awfully small gaps between some signals. Take a look at the
tracks going around the resistors and capacitors at the bottom of the board.
For a board like this, you could raise the track to pad spacing to 40 thou
quite easily. This will avoid lots of headaches in the future.
8) This is more a best practice than a rule, but have a look at the bottom
right hand corner of U2. Instead of just connecting two adjacent pads
together, I would recommend bringing the track into the open then going back
into the next pad, creating a "U" shape. This will help if you have to
debug the board. Currently, it would be difficult to see whether that
connection is a short or if it should be there without consulting the PCB
9) Carefully consider the position of your component identifications and
values on the silkscreen. Make sure that they dont fall on top of a via or
go outside of the bord boundary, you won't be able to read them after
manufacture. Also, try to avoid placing them under a component. Although
you can see them when you are assembling the board, you wont be able to see
them when the parts have been placed, making component identification
without the CAD drawings vary hard.
10) Finally, put some writing on a copper layer, maybe write what the board
is for. This will help you remember what the board is for when you pick it
up a few years down the line and it will avoid getting the top and bottom
copper layers mixed up during manufacture. Reversed text really stands out
when someone is checking a design.
I hope these tips help you to make the board more reliable and
More information about the Diy_efi