gEDA-user: Results of CustomPCB build of FLEX board

[Ben Jackson <ben@xxxxxxx>]

I had my Altera FLEX (obsolete FPGA I got a handful of for free) board
built by CustomPCB last week.  This was a trial run of using PCB for
professional manufacture, since I plan to do more complex 4 layer board
soon.

Overall I'm fairly pleased.  Gary Cho at CustomPCB answered my questions
promptly (if at odd hours, even for Malaysia).  When I accidentally asked
for a single-sided quote but included 2 sides with mask, I didn't get a
warning (beware, restarting firefox doesn't quite preserve forms!).  The
email confirmation of my order came very late Tue, Jul 10 with a promise
that the boards would ship by the following Monday.  FedEx actually made
their first delivery attempt that Monday (required a signature), so the
turnaround was faster than I expected.

Together, gschem, PCB and I combined to make a board that worked right
without any blue wires, so I'm also pleased with that.

Here's an image of one assembled board:

	http://ad7gd.net/flex/flex-build4.jpg

I did learn some important things:

(reference image:  http://ad7gd.net/flex/custompcb-detail.jpg   )

1)  Since I flooded GND on top and 3.3V on the bottom, every pad on the
board was within 'clearance' of some plane.  Since the many footprints
(including the 0603, 0805 and SOT-23 I used) footprints have the same
soldermask and clearance, any misalignment of the opening for the pad
exposed some adjacent plane, which is not good.  The long term solution
would be to fix all footprints to include some shrink for the soldermask.
Also, it would be good if PCB included a mask alignment tolerance in the
DRC parameters so it could both warn of potential problems and/or force
all masks to be at least 'mask tolerance' less than 'clearance'.

2)  Work with your PCB vendor on tricky footprints like QFP208.  After
I got the boards and found that the thin fingers of mask between the
QFP pads had been filtered out, Gary said they recommend a 8mil pad
with a 6mil mask (leaving about a 3mil gap around the pads).  The
QFP208_28 that I used has 11mil pads and <3mil of mask.  Also, only now
do I see looking at the text of the footprint that all of its coordinates
are on a 1mil grid, even though it's in a .01mil format and a metric part!

(I had no trouble soldering the QFP208 without a mask, in fact it
looks nicer than some of the 1206 stuff)

3)  The board was built with 8/8 rules (mostly done with 8/10) but
"slivers" in the polygon of 6 mil all survived.  3mil didn't.  This
might be worth considering when I get around to removing the slivers
in the polygon code (currently PCB assumes arbitrarily thin slivers
will keep the plane connected).

-- 
Ben Jackson AD7GD
<ben@xxxxxxx>
http://www.ben.com/


_______________________________________________
geda-user mailing list
geda-user@xxxxxxxxxxxxxx
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user