Greetings Andy,
arader:
I’m going to re-do the board, this time without the demux/mux chips and the 4 edge connectors. It should be much easier to do the board with only an avr, 2 shift registers, and the LED matrix.
Another approach is to have two PCBs. A second two-layer
PCB is actually cheaper than a single four-layer, everything
else being equal. The second PCB can piggy-back on the
first, effectively doubling the available area.
arader:
A few questions then before I go again. What exactly do you mean by “off grid”?
Before CADCAM tools the PCB design was done manually
with “analog” tools (Sticky tape and mylar sheets, followed
by photo-reduction in a technical camera). As an aid the
drafting light-table was covered with a precision 100mil
(0.1 inch grid). Keeping parts on the grid made the process
much easier to maintain, etc. The first round of pick and
place automatic assembly tools were also designed for
100mil steps, and of couse most electronic parts had been
redesigned with 100mil lead spacing.
With CADCAM we use the computer to store the “data”
instead of the analog artwork, so the grid concept is
less important.
Having said that, I strongly suggest sticking with 100mil
pitch. Its somewhat coarse by today’s standards, so
using 50mil or 25mil is also wise. I found your first
PCB to be on 5mil pitch, suggesting that parts were
nudged off the 100mil meridians.
arader:
I know my part placement is pretty random, but I would have thought with SMD parts there isn’t really a concept of a grid? What does it mean to be “on grid”?
I found the opposite to be true. SMT parts don’t have
holes, so the origin of the pads is taken as the
geometric centre. I found my first designs with SMT
to have lots of DRC errors! To further complicate things
the SMT footprint area varies for the same size package
depending upon the soldering method. I had to redraw
some SMT parts so that I could use a soldering iron,
where the part’s footprint was desinged for IR reflow.
arader:
Also, it sounds like what I’ll want to do this time around is put a ground pour on both sides before anything else, run the +5V lines to the parts, and then proceed with the remaining traces. Is there anything else in there that should be done in a certain order to make it easier?
I think that the NEWS placement of the connectors is a
problem, and I’d suggest moving them to be parallel
and nearer the centre of the PCB. From there you can
shorten many traces by “gate-swapping” and IO pin-swapping.
As most of the parts are SMT, the majority of the traces
will be on top (unless you flip some ICs to the bot side).
So making the bot layer a continuous plane and carving out
areas when a signal trace is placed on the bot layer.
The single plane can be split to form islands of ground
and supply.
If you remove the interface parts and leave the LED
drivers and uC you can add a second piggy-back board
for these later. By adding mechanical holes in the
corners you can attach the boards by standoffs. Or,
pick a mating connector that serves as both a mechanical
and electrical interface. Should be possibly to find a
common type that serves as a cable connection to
one PCB or as the bridge to another PCB.
This complication is only justified if you can’t get everything
on one PCB.
Comments Welcome!
I don’t think this would have been nearly as fun if I didn’t have you guys for advice!
