This is a pair of symbols, and a footprint for the card edge of expansion cards & cartridges.
This library is available as a KiCad module, that you can install with the KiCad "Plugin and Content Manager". I suggest doing so. I suggest including this repo as a git submodule within your project. Look for the latest release in the "Releases" section of the Github project.
I'll keep things stable in here. I'm about done adding stuff, and then it'll just be tweaked to fix errors.
The mating card edge connector on the X16 is the TE Connectivity 1-5530843-8. The card edge footprint matches the suggested layout of that part's data sheet. I also sanity checked it against the appearance of various ISA cards I've got. Per the data sheet, and PCB manufacturer recommendations, there is space at the bottom of the card edge for the bevel to be routed away. That's marked by a keep out zone, which disallows everything, since it'll be machined away.
The connector is about 0.4mm narrower than the data sheet suggests. That is to allow for PCB manufacturing tolerances while staying under the suggested width. And it made the width a whole number. Having handled the prototype card, I hope that this will make cards designed with this footprint easier to insert.
The footprint includes a number of user drawing lines.
- Distances to the rear and front of the motherboard
- Two heights ("low profile" and "full height") are marked along the rear end of the card. "Low profile" is the height of the TexElec prototyping card. "Full height" is what I think you can safely get away with before you should start taking your own measurements of whatever slot cover you're going to use.
- The rear end of the card has a number of lines indicating what space you've got available to go below the top of the card socket on the motherboard.
- I suggest not going below the top of the socket on the other side, as that will require 3D reasoning to ensure you remain clear of C53 (a tall electrolytic).
Most of the above applies to the cartridge as well. Confirmation of dimensions was carried out with a blank case purchased from Muramasa Entertainment.
Be aware that the front copper layer faces DOWN relative to the CX16 motherboard, not up as one might assume. The footprint is designed assuming the front of the cartridge case will face UP.
The cart has more of the board edge defined, including an internal hole. There are also a number of keep out zones defined, for places where the case comes into contact with the PCB for retention purposes.
The top edge of the board is missing from the footprint, so you may make a board of minimum height, or longer if you wish. The reasonable maximum is marked on the user drawings layer, but you might have larger cases available to you, or you might machine away a portion of the case and have your board extend out. (Connectors? A display? I look forward to seeing what you come up with.)
Keep in mind your limited vertical space. There is approximately 11.8mm of total internal height for board; I think it is divided about evenly between the two sides, but I made no attempt to measure this. Certainly if any of your components exceed ~4mm in height, you should take some careful measurements and do some prototyping of your own.
There are two symbols, the main one is the "physical" symbol, where all pins are positioned to correspond to their physical pin. The "Alt" symbol rearranges things, so that groups of pins are in order, the groups have a small separation between them, and the duplicated power pins are on top of each other. (This tells KiCad that they're all the same net, and reduces the number of lines you've got to draw.)
The IOx pins are driven by a 74ACT138, making them active low signals. I've added bars to their signal names to reflect this. I realize that the 6502 derived signals use a "B" to indicate that they're active low, but I'm leaving them be to better match existing 6502 docs. The X16 docs don't mark the lines with any character, so I figure the bar conveys the information best while ensuring nobody goes searching for the "IO4B" signal and wonders why they can't find it.
The AUDIO_L and AUDIO_R pins are marked as bidirectional, because those pins are connected to the summing node of the system mixer (through a resistor). An expansion card could choose to "listen" to that signal, or emit audio of its own into that node. The VERA and YM2151 outputs are buffered by TL074 op amps before being fed into the overall mixer. If you want to emit audio, you might do the same. Please keep in mind that other expansion devices might be driving these pins directly with op amps. Consider putting a resistor between you and the bus, so as to avoid your amp fighting another amp. Or your device being back-driven by another device's amp.
Finally, while the SDA pin is bidirectional, the SCL pin is marked as an output of the edge connector, to match the KiCad convention of I2C masters having SCL as an output. (This is despite the ability of I2C slaves to stretch the clock signal as necessary.)
This is a simple symbol intended to be used with a right-angled 2x5 female header, to make a little board that sticks up from the motherboard. Something like the Würth Elektronik 613010243121.
Same idea, but you'd need a larger connector.
TODO
- The extra 65C22 pin header doesn't have enough to support a complete device (no power), so I don't consider it interesting enough to bother with.
- SNES 3/4 really only has one thing you could do with it, which is bring it out to some more controller ports, so there's not much reuse value for a symbol.
- Front panel should just go to LEDs via cables, not much sense in one larger connector to it.
- For the VERA header, I'd sooner make a symbol representing a place to plug a VERA into, to encourage reuse of them in other applications.
I've had the cartridge footprint manufactured, and it seems to be fine. Everything here remains use-at-your-own-risk, of course, but I will be using them without hesitation going forward.
If you spot any errors, please report them. PRs welcomed. I do ask that you make a point of including evidence for any dimensional changes.
You might be interested in the following:
- https://www.kicad.org/
- Consider donating to KiCad if you find it, or this library, useful.
- https://github.com/Alarm-Siren/6502-kicad-library
- RetroLib, a KiCad symbol library for 6502 and related retro microchips