Paul, The drawing does not show actual trace width.
Yoda, Those shorted pins above the 5V regulator are for an optional 12V regulator. I agree, the 5V reg should be moved a little right.
Dave, Yes, the holes are close to the edge (aren't we all?).
Right, great questions, let me describe the board.
All the traces between the S-100 and Buffer IC's are 12mil with 13mil spacing. Traces that tie the 74LS245 chip directions to ground or vcc are 8mil. The board is ready to go as a slave board (ie memory, i/o, etc). If you need to convert it to a CPU board, the buffer directions need to be reversed, the 8mil traces need to be cut, jumper wires added. The +5V and Ground traces are 50mil, they extend up the right side of the board and feed every 4th hole (only the top layer is shown, the GND is fed to every 4th hole from the copper side). From these holes, bus wire can be used to feed a row of 300mil chips. The +8V is also 50mil to the regulator, but goes through a short 25 mil "fuse" trace. This way a short will not fry the whole trace and damage the gold plated S-100 pads. The +16V and -16V use 35mil traces and go through a short 25mil "fuse" trace too (I should reduce this to 20mil).
The 5V regulator is at the same location where Andrew placed it on the Unbuffered board, but I agree, it should come a little to the right, say 100mil. Above it are provisions for a +12V and -12V regulator. The power traces reach those pads, but you don't have to use them. There's plenty of holes around it so you can easily install any other IC there around the specialized holes for the regulator. This regulator does not need to move, it will never require a big heat sink... I hope.
The top row can be made like this, but I agree it's a little too close... I think I'll shift everything down 50mil and sacrifice a row on the bottom.
The 74LS245 chips can be placed side by side (even on sockets). I've checked this out with a dozen different chips from my junk box, it works for all of them. I think the 14 pin chips have this problem, especially those from 1970's. I can redo this test and take photo's if that helps?
Oh, the other changes I've made to this board from Andrew's board is. I've upped the pad size to 64mil (from 60mil) and decreased the drill size to 38mil from 42mil. This gives more pad for soldering. 38mil is good for .025 square posts and wire wrap sockets. I even checked some 10W resistors, their leads are .036. I know my guy will give 38mil holes, I believe he drills 40mil and plates 1mil, but he will be within 1/2 mil of the 38.
Regarding the holes, should I go back to 42? 40? or is 38 good for you?
> Subject: Re: [N8VEM-S100:2570] Re: Board Run: Unbuffered Prototyping
> From: frave...@gmail.com
> Date: Fri, 28 Feb 2014 09:28:18 -0500
> To: n8vem...@googlegroups.com
> I would pull that top row of holes; you're going to be way too close to the edge. Sometimes the DRC is there for a reason... A lot of the design rules are ones that PCB manufacturers will also call out because they can drastically reduce yield. Holes that close to the edge are likely to end up cut through if the board is misregistered at all, and a lot of board houses don't like you putting the pads so close to the edge either.
> - Dave
> On Feb 28, 2014, at 3:44 AM, Crusty OMO <cru...@hotmail.com> wrote:
> > I don't know if the .pdf made it... let's try inline picture....
> > <SeaoPTH.JPG>
> You received this message because you are subscribed to the Google Groups "N8VEM-S100" group.
> To unsubscribe from this group and stop receiving emails from it, send an email to n8vem-s100+...@googlegroups.com.
> For more options, visit https://groups.google.com/groups/opt_out.