I figured while I am on a roll, I might as well try my hand at making the power-board for the C64 Optimized PSU. Thought I would offer it up for suggestion, or if anyone else wanted to use it! I could probably clean up the traces from the +5V to the voltage regulator but I didn’t want to make any assumptions.
Enjoy! Flames welcome!
[c64psu.zip](< base_url >/applications/core/interface/file/attachment.php?id=4346)
[c64psu.pdf](< base_url >/applications/core/interface/file/attachment.php?id=4347)
Flame: if you include a screenshot it makes it about 10 times faster for me to read the png/gif/whatev, than to open a pdf reader and wait for it to render. PDF is needed for dimension-accurate printing, not really anything else 
for power lines wider tracks are advised
for power lines wider tracks are advised
I thought about that too (for both this one and the BankStick board I’m working on). How much larger should I make them? I used the default of 0.016, but have plenty of room on this board to make them bigger.
One question I had - when I route the +5V to the 7809, can I jump off the + of the 16V capacitor? The C64 Optimized PSU schematic shows the wire to be before the capacitor and not after, but can I go up to the capacitor? Reason being is that I might be able to tidy things up further if I can do that.
Flame: if you include a screenshot it makes it about 10 times faster for me to read the png/gif/whatev, than to open a pdf reader and wait for it to render. PDF is needed for dimension-accurate printing, not really anything else
Haha. Fair enough 
You got me. I was being lazy
Haha. Fair enough
Hahahah really? I often give sceenshots cause I’m too lazy to make a pdf 
Well, on the Mac, it’s easier to print to PDF I find
Speaking of, though, here’s the updated version! Bigger wires and in a format friendly for BatchPCB (http://batchpcb.com). The only problem I am having is the that the Design Rules says the Stop Mask is wrong. Not sure how to fix it, but BatchPCB’s own DRC doesn’t seem to be complaining about it. *shrug*
[c64psu.zip](< base_url >/applications/core/interface/file/attachment.php?id=4350)
I don’t quite see why you have all the text on both the tNames and 121_tsilk layers. Unless that’s a batchpcb thing, it’s not really a good idea The errors you get mean that there’s something within the stop masked parts. That would be all the component outlines on tPlace. Hide the layer and run the DRC again, and you’ll see.
You’ve done some things in the layout that I cannot quite see a reason for, which isn’t necessarily bad though
Footprints of 100nF/330nF caps tend to be 200mil - you might wanna check the parts you plan to use.
I made some changes to the layout (the caps are supposed to be flat as in parallel to the PCB) kinda answering one your questions: Yes, you can route the signals like you asked. Why wouldn’t you? As long as the parts are on the correct net you can basically wire them however you like (this is a half-truth. While theoretically you can, you wouldn’t want to do it for various reasons. A bypass cap that is supposed to smooth things out for an IC don’t help much on the other side of the board, HF traces (and all others really) should be as short as possible, well you get the idea). Before you start actually laying down traces, move the components around press F6 and see how the airwires change. That’s another way of looking at the answer to your question ;D
I just wanna highlight this tip, very important step for pcb cad newbies.
Before you start actually laying down traces, move the components around press F6 and see how the airwires change.
Wow so much awesome information! Thanks nILS and stryd_one! I’m not sure where to start, so I’ll jump right in:
I don’t quite see why you have all the text on both the tNames and 121_tsilk layers. Unless that’s a batchpcb thing, it’s not really a good idea
They actually require layer 29/30 (tStop/bStop) as well as the silk layers (they are created with a script that recommend running). The errors are actually for layer 29, and, you’re right, if I hide them, there are no errors. Since their DRC step passed on their end, I assume it’s probably nothing to worry about?
You’ve done some things in the layout that I cannot quite see a reason for, which isn’t necessarily bad though
Whoops Can’t say I’m too surprised since I’m a fairly big PCB CAD newb
Footprints of 100nF/330nF caps tend to be 200mil - you might wanna check the parts you plan to use.
I sort of guestimated based on the caps I purchased for the protoboard design of the board. They are the ones that stand up and are usually round at the top. Sort of like a stick figure without arms. Radial I think? The symbols you have are for axial right? Or no?
I made some changes to the layout (the caps are supposed to be flat as in parallel to the PCB) kinda answering one your questions: Yes, you can route the signals like you asked. Why wouldn’t you? As long as the parts are on the correct net you can basically wire them however you like (this is a half-truth. While theoretically you can, you wouldn’t want to do it for various reasons. A bypass cap that is supposed to smooth things out for an IC don’t help much on the other side of the board, HF traces (and all others really) should be as short as possible, well you get the idea). Before you start actually laying down traces, move the components around press F6 and see how the airwires change. That’s another way of looking at the answer to your question ;D
I think I see what you are doing. So basically, it doesn’t matter if I connect the +5V with the -9V right at the big capacitors? I didn’t think so, but didn’t want to waste a board design trying to find out. So thanks for clearing that up, though I was wondering if you can elaborate on what you mean by parallel and what lengths should be short as possible? Do you mean all lengths or, in this case, the small caps? If all lengths, now that I can connect the wires to the big caps, I can shorten the circuit even more. Actually, your board design is most of the way there it looks like
F6, by the way, didn’t work. That turns the grid off and on for me, but I assume you are referring to the RatsNest feature? I used that on a regular basis, but in this case, I wasn’t sure if I could trust how it connected the wires since I wasn’t sure about when I could combine voltages as noted above.
Finally, I noticed that you used a ground plane. I had considered doing that (just like with the Bankstick board I’m working on) but I was a bit confused about how that would work or if I needed it for a power board. I probably should’ve thought about it more, since your solution looks obviously exactly like it should look 
I assume the general rule of thumb is to ALWAYS use a ground plane? And probably almost always use an isolation plane for a two layer board?
Ok, I applied some of the suggestions and have an update! I was able to cut down the size a bit more too by changing things around. The only thing I have yet to do is look at switching to the parallel mounted capacitors (I think I confused myself on the issue in my last post :). The ones on my version should be vertically mounted (radially?).
Anyways enjoy. Flames welcome
I assume it’s probably nothing to worry about?
Correct.
I sort of guestimated based on the caps I purchased for the protoboard design of the board. They are the ones that stand up and are usually round at the top. Sort of like a stick figure without arms. Radial I think? The symbols you have are for axial right? Or no?
Guessing is not good enough Check the components that you want to use. Stick figure without arms… Yes, um, how about a link to a picture? I used special footprints that allow to use both 100mil and 200mil caps.
though I was wondering if you can elaborate on what you mean by parallel and what lengths should be short as possible?
Well, basically any trace should be as short as possible, but not any shorter. Parallel traces are bad as they introduce crosstalk, but don’t hurt in a lot of cases.
F6, by the way, didn’t work. That turns the grid off and on for me, but I assume you are referring to the RatsNest feature?
…which is mapped to F6 on my eagle. Whoops
Almost. If you have mixed analog/digital circuits like the SID module you might want to separate the Ground planes or not have one in certain parts. Generally you do want one and you also want an isolation plane.
This is the type of capacitor I am referring to:
These are called radial, yes.
The other type you mentioned, axial, is usually referring to an electrolytic cap, where the leads are located along the axis of the ‘can’ package.
These types of cap are a lot less common nowadays (outside of the valve amplifier realm).
Ceramic caps in the nF range tend to get rather expensive. I’d go with polyester film caps like the WIMA MKS or the likes. Something like these:
Thanks for the clarification, /tilted/! I think I get it now. Your (nILS’s) board layout IS for radial caps, but you are allowing for different sizes?
As for the caps, I’ll keep those in mind. The place I often get parts from (Allied Electronis) does not appear to have many of the ones you mention in stock though 
But I’ll keep that in mind. I really like to use them since they have no minimum order and are SUPER fast due to where i live in relation to them.
That said, do you perhaps have a part number from another site and/or link?
Your (nILS’s) board layout IS for radial caps, but you are allowing for different sizes?
Exactly. If you look at the footprint you’ll see it has 3 pins. Two of which are directly connected. So you can put different sized caps in there. Kinda like what you see in the attachment.
That said, do you perhaps have a part number from another site and/or link?
I usually order from reichelt or conrad. Seeing that you are in the US this is not really gonna help you
m00dawg, are you considering running a PCB bulk order for these? I know it seems trivial since it’s such a simple circuit, but for a lot of the newbies, it might come in handy. If not, I think I’ll try my hand at DIY etching using this design. Always wanted to give that a try.
While I’m at it, I might try using the same etching technique for a Front Panel, as well…maybe go for a steampunk look. See this article.
For a bulk-orderable version I’d definitely go with more options for the footprints, … For a DIY etch version I’d definitely go with bigger traces, bigger holes, bigger pads, … If there’s any interest I’d be happy to put together a layout for either option.
If there’s any interest I’d be happy to put together a layout for either option.
Thanks, nILs! My guess is that there would be interest in two PCB versions:
allows room for desoldered C64 power port, switch and the two DSUB ports for banksticks, along with the metal facing that is removed from a C64. Along the lines of what Daniel Price did for his OPSU.
Simple version like m00dawg is designing for those not using C64 parts or a C64 case.
I would definitely be interested in a self-etch version that uses the C64 parts. Any assistance I can provide, just let me know (measurements of C64 parts, etc..). I’ve never designed a PCB, so I’m following this thread closely to learn. I would use the design to etch a board and post feedback on the forum for others to follow.
