osiweb.org

OK, I have a little breathing room, so I finally had a chance to look at this. My Eagle skills are rustier than I thought. I have been spoiled by Altium.

Philip, I have taken the liberty of re-arranging the schematics to be a little more clear. However, thanks for taking the initiative to get this going; this has been on my to-do list for a while. The schematics are distributed over three sheets to decompress them a bit. The file is here. A few notes:

• I didn't include the MOTOR ON switch; I don't see a need for it. It would be easy to put a jumper back, though.
• Three of the 7486 XOR gates were just being used as inverters, and the fourth was being used essentially as an OR of the /HEAD LOAD and /STEP lines. A NAND in the same configuration will do the same thing, so I substituted a 74LS00. I also substituted a 74LS00 for one of the 7438's (used in the data separator, and gating the /INDEX pulses), since these are just driving local TTL, and don't need to be buffers. These two substitutions provide more flexibility for gate and part swapping to simplify the board routing.
• I added a second floppy connector

I haven't yet started routing the board. I will be out of town over the weekend, but will do the routing when I get back. I had thought about just replacing everything with a PIC chip, since it seems crazy in 2012 to use so many small gates, but ultimately it's better to have a piece of hardware that reflects the times of the original. This data separator, with the 6ms data window after the clock pulse, is pretty classic for single density drives at the time, across multiple different computers; I've seen an almost identical circuit in an old Ciarcia's Circuit Cellar article on a TRS-80 floppy interface.

Dave

Great!
It sounds like you've revamped the circuit quite a lot. Unfortunately your link to the file seems to be dead, so I can't see what you have done.
I'm excited to see the changes, and excited to see this project progress.

Thanks
Phil

Whoops, I messed up the upload. Just go back in town and re-uploaded the file here. Please check for errors. Any suggestions are welcome! I'll let it sit a day or two for comments, and then I'll go ahead and lay it out. It should be a quick layout.

Best regards,

Dave

Latest cleanups and routing posted here. Out of laziness, I used two ground planes, laid the 5V circuit, connected up the floppy connectors, and then invoked the auto router, which did did get 100% routing, but REALLY ugly. Many of the tracks were acceptable, if convoluted, so I cleaned up the rest, stitched together the ground planes on both sides, added ground path shortcuts near the signal vias, etc. Next time, I'll just do the whole thing by hand.

Although I started this with Eagle 5.11 (full edition), I downloaded Eagle 6 to try it out, and the whole thing got converted to Eagle 6. Since I'm not sure I want to upgrade, I am using the free edition. It still seems to work fine with this 3"x4" 2 layer board, but doesn't allow adding new components on any sheets above 1. You can get around that by placing them on sheet 1, then cutting and pasting.

Dave

I upgraded to Eagle 6.0 so that I could view your files too.
I have to admit that I can only really look at your schematic on a very superficial level as I'm not really good at circuits! So I'm just going to have to have faith in your superior skills and assume the logic is all good

However, It looks great to me. I see that you now have selectors for the ready signal, drive selects and have also removed the test pin in preference of what looks like a large pad area. I'm curious why you opted for the pad over a pin? I would have thought a pin would have been easier to hook a probe on to.

Anyway, I think it all looks really good. Running the 'errors' check in Eagle shows some overlap and stop mask errors, but I don't know if these are anything to work about.

Cool stuff.

You must be pretty decent at circuits. You seem quite comfortable jumping in and repairing these old machines.

I hope the logic is sound I didn't really change the logic, so hopefully it will work out. Since I was unable to break out the machine to test it on, I am relying somewhat on faith. However, the data separator is a pretty widely published and used design, by John Hoeppner, who was one of the floppy gurus at the time.

I decided to swap the test point for a surface mount version that I have found to be more convenient to work with, in practice. Perhaps it would be good to put a couple of vias adjacent to it, to solder a u-shaped piece of wire as an alternate.

I thought I had got the overlaps out, but may have moved something. I will make sure it's clean before sending it off. The stop mask errors weren't reported with version 5, but are reported by version 6. They are due to the silk-screen lines over the pads, mostly in the library parts. That would be too much work to fix, and the boardhouse will just leave defects in the lines over the holes. I was going to put them in the "approved" list, but with 200 of them, it was taking too long, so I opted to ignore.

I'll check it over this weekend, and send out the design files.

Next board will be a direct copy A15 I/O board replacement. Philip, is there a way to make an accurate DXF file from photos of the front and back of the A15 board? I'm trying to figure out the best way to go about reproducing some of the boards, and an automated method to create DXFs would accelerate the process, but I'm not so familiar with the various graphics programs, with that being your specialty (as I understand), I'd be grateful for any guidance.

Best regards,

Dave

My only thought about a pad is that because the board is in a very tight space then it may be very difficult to get a probe in for testing, a couple of VIA's would be great.

As for the A15 board, I think it could be hand drawn in Illustrator and using some software converters to convert it to DXF (http://www.baby-universe.co.jp/en/plug- ... exdxf-pro/). I'll do some test with the conversion from .ai to DXF probably with the A14 drawing I have already done (could we get a few of these made too?). The difficult part would be the time it takes to draw it all up by hand. If you like I give it a go, but it may take a while. Getting decent scans of an original board would be most important.

Phil

Hi Phil,

Definitely, if you can convert the board you already made into DXF, I can turn it into a set of gerbers and have it made.

For new efforts, I was hoping there might be a way to automate the process; for example, use photoshop to accentuate the traces, then turn into a black & white image, touch it up by hand, then automatically extract the outlines, convert to vector format, then export as DXF. If hand drawing were involved, then it would be best to find a way to do this directly in a capable ECAD program. I will explore if there is a way to do it with Altium; for example, import a bitmap into a mechanical layer, then trace it out on a copper layer.

Dave

dave wrote: I thought I had got the overlaps out, but may have moved something. I will make sure it's clean before sending it off.

Those overlaps are due to a couple of "net ties" I placed. Instead of tying unused gate inputs directly to ground, I insert a "net tie", which is like a zero ohm resistor made out of two pads and a trace connecting them. That way, if the gate is ever needed for a mod or blue-wire fix, you just have to cut that trace, and you can jumper directly to the input.

Eagle complains because in the schematic, the two pads on the tie are on different nets; but on the PCB, the copper is connected. It's good that the PCB program detects it. That is why Eagle has an "Approved" list--so that intentional or acceptable rule violations can be approved, and warnings will be suppressed. I'll add these to the approved list.

One thing I forgot to mention is about the variable resistor for tuning. When I was making my parts selection I saw there were a few different types with different leg configurations. Some had a triangular distribution and others had the legs in a straight line. I selected the one in a straight line, and I see you are using the same. I'm not sure which was the better or more popular and easier to source. Just though I'd mention it incase I chose a very obscure part.

Philip