Spent the day building two r8c-based boards, thought I'd give a quick status, since I did some new things with this.
First off, I've got a board that has a USB chip (FTDI232R) connected to an R8C/20, connected to a bunch of headers. In other words, it's a programmable USB GPIO port. The only design flaw so far is that the mini-B connector has an extra pin, and ground is on pin 5 instead of pin 4 like all other USB connectors. Fortunately, pin 4 is not connected on the device end, so I just shorted pins 4 and 5, and it worked just fine. Haven't talked with the R8C yet, I need to adapt my R8C programmer to the FTDI driver. This board also used the global puller, as I was able to coerce it to give me useful results. Second, I've got an R8C/27 (TQFP-32) adapter (files are at http://www.delorie.com/pcb/r8c-27-adapter/). Along with being a TQFP to DIP converter, it includes some pullups and the oscillator, so aside from programming you shouldn't need any support parts. This board takes advantage of the ability to rotate parts 45 degrees. Now, for the new things... The DIP adapter is a two-layer board. However, I did it using two separate SS boards, taped together. This lets me line up the two etched boards after etching, instead of before etching. The clad is 16 mil (1/64") with 1 oz copper, resulting in a 36 mil board. The tape is 3M 7953 laminate adhesive, about 4 mil thick. The USB board is a home-etched four layer board. Yes, four. The core is a 32 mil DS board, where I lined up the resist before etching. What I did here is iron on one side, drill out the alignment holes, and use those to line up the resist for the other side. This core held the ground and power planes. Then I taped the outer layers to it. Those were 8 mil 1/2oz SS, and are pretty much transparent, so easy to line up and tape on. The tricky part is the vias. What I ended up doing is drilling big holes in the outer layers before taping them on, then drilling small holes through the full stack. That left some of the inner layer copper exposed through the holes in the outer layers. For signal vias, I only did the small holes, like a 2 layer board. If I do more of these, I'm going to have to add some support to PCB for it, because I mis-drilled a lot of the holes. For example, to connect a top signal (layer 1) to power (layer 3), I had to drill a big (35-45 mil) hole in layer 4, and no hole in layer 1, then a 14 mil hole through the stack. To connect it to ground instead, I drill a 22 mil hole in layer one and no other holes. To connect both sides to an inner layer means drilling a 22, a 25, and a 14 mil hole. Plus, it would have gone better if I could have had different size copper (or no copper) on different layers based on connectivity. I had to print each layer separately, because PCB wouldn't let me paste two boards into one layout and flip one, which would have let me etch both sides on one board then cut them apart and tape them together. I also tried using glossy magazine paper instead of my usual coated TT paper. I wanted to use some of my 64 mil (1/16") clad that won't fit through the laminator, too, so I ended up ironing it on. The paper rubbed off like "they" said, but I was back to the original problem of getting the toner to stick completely, without getting so hot it smears. I think the paper might work in the laminator though, and I have more clad than coated paper at the moment. _______________________________________________ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user