[personal] RE: Experience with ECB bus?

----- 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? 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. Comments - 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 connector. 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 after. Best regards, Mike Hatch Web - www.soemtron.org Email - mike at soemtron.org Looking for a PDP-7 (some hope!)