How do I create a PCB with an edge card connector?

I’d guess it is fairly rate these days. It wouldn’t be hard to make a part for this it is just a series of fingers with a particular spacing. The fingers are however typically gold plated which is both more complex (you used to 30 years ago, have to short all the fingers together in your footprint to allow the gold to be plated on, don’t know what the case is these days). If you have the specs for the edge connector I can make a part easily enough.


I don’t necessarily need the fingers to be gold plated.

Here is the electrical signal pinout:

Here is a typical proto board:

I find this, which describes the physical dimensions:

“The standard Apple II Slot card has 50 contacts, 25 per side, and is up to 2.75” high
(not counting contacts). Contact spacing is 0.10". Length varies. About 0.50" of the length
can extend beyond the contacts toward the back of the computer.
You may be able to find an ‘Apple II prototyping board’ from a surplus parts seller;
however, these boards are no longer a standard item. To get a new board, you will
probably have to get a PC ISA-8 (“PC XT”) Slot board (or an ISA-8/16 Slot board
with the extra contacts trimmed off).
An ISA-8 board has 31 contacts per side spaced the same as an A2 card. From the
edge facing the front of the computer, you will need to count down and trim away 6
contacts (per side). It’s best to use a real A2 board as a guide to determine pin centering
and to decide what to slice off for a good fit in an Apple II Slot. A Dremel tool with a
sand wheel is good for this sort of slicing."

The spacing and depth are the same as the IBM PC ISA slot, (the J1 part of the below referenced picture) the Apple II just has 50 pins instead of 62.

Is that enough to make the part? I greatly appreciate your kind offer of help. I’ve been using Fritzing for breadboard projects for a while but I am just trying to ramp up to building PCBs.

You do actually need the gold plating very likely (although I’m far from a current board expert, and one of our better board makers may have a suggestion) as bare copper tarnishes and won’t be left anyway, if the solder mask is blocked out, the edge pins will be by default covered with solder as contacts ready for soldering. This is not good for the connectors on your apple 2 and will possibly damage them. A search for “apple 2 prototype board” on ebay turns up two suppliers (the cheap one with only one board left for about $20) that have boards. I expect that would be a better bet for you. I’d wait and see what more experienced board makers think about edge connector pins without gold plating (and if Fritzing can do whatever is needed for gold plating) and get a quote from a board house for gold plating (as it may be $$$) before trying this. In fact a google search on “apple 2 prototype board” turns up several suppliers which I expect are a better bet (as the look to be gold plated as they should be). Even if you buy one you may still want a Fritzing part to document what you put on it, but that is easier than trying to actually make a pcb view that could be fabricated.


I’ve got plenty of proto boards. Some have plated connectors, but most don’t. Even back in the day that was common. I’ve seen production boards that didn’t have plated connectors and some of those have been in use for decades… Anyway, I’ve got designs that I’ve built on proto boards that I’d like to make some probably limited size runs of for other people. I don’t have the time to hand solder on a proto board for that. It will be time consuming enough assembling boards on a proper PCB. This is more of a labor of love than anything, because there is no profit in any of this stuff. I’ll be lucky to cover my expenses and all of my labor is not going to be compensated. I’m also learning a lot from it of course. I probably won’t ever profit from that either… but it may make my resume a little more interesting.

Anyway, any help you can give in terms of making the part will be greatly appreciated.

OK I can make a part easily enough. It would be useful to have the outline dimensions of the card, height width and especially the offset from the edges to the two edges where the edge connector goes in and the depth of that slot. The edge connector data sheet should have the appropriate footprint for that part but the spacing of the offset is also critical to success.


I can not say I know much about edge connectors being used in sockets but I do have a lot of boards manufactured so maybe I can add a little to the conversation. From the place I get my boards made you get the choice of HASL, HASL (lead free), ENIG (immersion gold), Bare copper (by request) and Hard Plated Gold (for Fingers by request). Of those obviously the Hard Plated Gold is ideal but I think the ENIG would be fine for a board only being inserted once or twice. Even the HASL ones would be fine as they do not oxidize like bare copper.

To clarify… I’m not wanting to make proto boards. I have designs for a few boards I want to build, a WiFi card, an Ethernet card and a USB storage card to begin with.

I only need the edge card connector, I’ve got figured out the rest of it. Most of the other stuff I’m using is simple off the shelf stuff that is easy in Fritzing… 74LSxx TTL logic chips, M2716 EPROMs, IDC header connectors, etc… So stuff that uses DIP sockets and that stuff is no problem.

About the only thing I find is that many of the chips I am using don’t have pre-defined parts so I am having to enter the pin names, etc. Is any of that stuff that other people could use? I am assuming that the basic 74LS (and HC or HCT) chips, EPROMs and common interface chips like the 6522, 6551, etc. are still used for other things so someone else might benefit from not having to re-invent them? Or maybe only useful to retro-computing enthusiasts?

google is your friend here, “fritzing part part_name” will sometimes turn up a part someone else has made. If it doesn’t and you make one (either generic or full) by all means share them at least in the forum for others to use.
The first edge connector on digikey that I found with a pcb layout

shows .40 depth of the connector, does that match with the proto boards you have? I expect I’l make a part for just the edge connector and leave you to be able to set the board dimensions to whatever you need. It sounds like you have plating options, so I’d recommend looking at them to protect your edge connectors.


I should also say I have made edge connectors for soldering small boards to each other at 90 degrees and for my part I had to make an SMD part and then use it on both sides because THT parts all get holes in them. I did then place vias on every single finger to ensure both sides were connected.

I am attaching my edge connector part in case anyone wants to use it as a start for these connectors. I repeat, this one will not work for what you want but may speed up development. 20 Pad Edge Connector.fzpz (7.2 KB)

Thanks, every little bit helps, I was just realizing that a standard tht part usually has holes and was starting to think about how to do that …


Yeah, I googled a bunch of the parts I use, and got nothing on most of them. I will share the ones I’ve entered in case anyone else can benefit from them. It is only a few so far, but it will probably be a bunch more 74LSxx chips, a few 4xxx series CMOS chips and some 65xx and 68xx I/O chips at least.

That edge card looks pretty close. I don’t have a card handy where I am now to measure it. I think as long as it is deep enough it is O.K., a little too deep won’t hurt. The ISA card image I sent shows what I believe is 7.62mm as the depth which is .30", but I can’t imagine .40" would hurt anything.

Thanks! That does look like a promising start!

I’m experimenting with a 2 pin generic header to see if by creative editing the fzp file I cause it to create a pad on top or bottom (selectable in the fzp) that will connect to a through hole pad. If not then the two smds will be the answer but it would be nicer if it can be done as one part (but I’m not sure it can yet).


Can you make a pad on the end without a hole the same dia as the track width. The pad would connect and wouldn’t be seen.

I think I remember old floppies with edge connectors being plain copper., and ISA cards just being tinned.

The tricky part is going to be to connect to both the top and bottom traces of the connector to different through hole pads (because the same pad on each side of the board is a different connector). With copper0 under copper1 the thru hole connects both pads which isn’t what we want. I remember some of the old Sparkfun parts with separate copper1 and copper0 with the connectorpad in one view and a circle in the other which I think is still supported as legacy, but I can’t right now find one (of course). If that still works I think it should be possible to do this as a single part with the same pads on both sides going to different through hole pads which is what we want in this case. A test with just creating copper0 and copper1 as same level groups with a connector1pin in copper1 and a circle in copper0 doesn’t work in Fritzing so I need to find one of those old parts to look at what they did. By editing the fzp file I can get a trace only in copper0, but the one for copper1 still appears in both traces as if gets copied to copper0 even though I didn’t define that layer in the fzp. It will be interesting to see if I can convince Fritzing to do this …


Ah, hence your 2 SMD part idea.

OK here is the fast ugly hack version. Basically a smd part that has the 25 pins for the edge connector (available for part export from the temp parts bin with the fzz loaded) copied to the sketch twice, once on the bottom layer and once on the top layer. There are 25 vias all connected on the top layer, and one example via with clumsy routing on the bottom layer to give you the idea of what needs to be done there. The effect is that you (potentially anyway) all 50 pins available on both layers of the board. Now I go back to trying to figure out how to convince Fritzing to do this in a single part (which may or may not be possible). This should work, its just ugly.

apple2_edge_connector.fzz (14.3 KB)

when exported as gerbers and viewed it works as intended.
Schematic is OK, it appears as two sets of headers. Breadboard is less OK as it shows as two headers (which is what I cloned the part from). They should probably just be supressed which I haven’t done here.


Thanks vanepp, I will give it a try later!

The breadboard view probably isn’t that horrible, as that should be easy to hook wires to… I looked at the part and it looks good. I am going to try to add the rest of my parts to it and wire it up today.

Thanks so much for all the help. I hope that there will be other people who can benefit from this also.

This does look like the only solution for now. As far as I can see this is a design limitation on the current Fritzing version (which I will keep in mind for development). On this version you can’t have separate copper0 and copper1 layers which is mostly sensible but it does break this one use case and I think there needs to be a way to do this. I did find a part in core (the ATmega644) and I can mangle the fzp file to work on 9.3b but so far any change I make to the pcb svg with Inkscape breaks Fritzing (the connections no longer work for some reason). It did however turn up a couple of bugs in my parts checking script that I need to fix so the effort wasn’t wasted. The headers as output in breadboard is probably the best anyway. Any part with overlapping connectors (like right angle headers) is hard to represent accurately in breadboard and the current headers probably do as well as anything.