[personal] RE: Experience with ECB bus?
mike at brickfieldspark.org
Wed Jul 23 03:54:49 CDT 2008
----- Original Message -----
From: "Andrew Lynch" <lynchaj at yahoo.com>
To: <cctalk at classiccmp.org>
Sent: Wednesday, July 23, 2008 3:18 AM
Subject: [personal] RE: Experience with ECB bus?
>> Vcc and ground traces are triple wide (51 mils) minimum and also routed
>> both the component and copper sides of the board. The rest of the traces
>> are the usual 17 mils wide.
>> After I order some of these backplanes, I will make them available in a
>> similar fashion as the N8VEM SBC. The PCBs will be available for $20
>> plus shipping. The builder will have to source the rest of the parts.
>> If you are interested in helping or have questions, please review the PCB
>> backplane design at:
>> Thanks in advance for any *constructive* feedback. Have a nice day!
>> Andrew Lynch
Hi, just seen the post, I do pcb design for a living so here goes. I presume
the file is "printing backplane-brd.pdf".
If you have Gerber output I can view them directly and check hole/pad sizes
as the DIN connector hole to pad size looks to have big (oversize) holes.
I read you spec as - 2oz (70um) Cu, 3.2mm. 50thou track @ 1oz is good for
3.5A, 2oz 7A, Etc. 10thou track will handle 0.5A @ 1oz etc.
What is the plane to pad/track gap ?
Around the end connectors there are "fingers" of plane around the B row of
the connector, try altering the plane cut-out / limits / flood to remove
these as they will serve no great useful purpose.
The ground thermals are too wide, the thermal will not serve as a thermal
due to the width. Go one way or the other - reduce the width and set them at
45deg and you should get all 4 legs in, or make them solid.
Each ground thermal has a tiny (<10thou ?) routing "connection" presumably
for the net connection, try routing this over the actual thermal leg.
The mounting holes need not be isolated if your ground is at chassis, if not
you may need insulating washers under the screws.
Add identification text in the planes, name board # etc in small text, does
not detract too much from the functionality.
Could set the planes supply one side and ground the other, sandwiched planes
work better. However I would probably split the planes horizontally at about
pin 2, and make the area above pin 2 all supply plane, and the rest ground
plane. If you wanted you could then add decoupling on the board for each
Tracking to the indicator LED can be much smaller 10thou would be Ok.
Add a solder mask for both sides, should not add to the cost especially if
you use a company like PCB Train http://www.pcbtrain.co.uk/ (for UK and
Europe, must be something like this in the US), makes soldering a lot
easier, and it looks just that bit more "professional".
A lot there but all offered constructively.
At 4 - 10 Mhz a double sided board will not be noticeably better for more or
less plane, 4 layer would be better but I do realise the cost implication.
What sort of current is drawn by each board ?.
If you agree I'd like to see Gerbers, mail me direct, I'll destroy them
Web - www.soemtron.org
Email - mike at soemtron.org
Looking for a PDP-7 (some hope!)
More information about the cctalk