SNES cartridge PCB thickness

Hello all,

I've recently become quite interested in SNES and SNES hardware. I'm by no means an expert on the subject matter, thus I'm looking to learn as much as I can by starting up a small project. Simply put, I'm looking to drop a nice FPGA chip into a game cartridge, and using it as a learning tool. I wont go into the details but I'm looking to get a PCB board manufactured. The issue is, from my searching SNES cartridge PCB boards are 1.2mm thick, while 99% of PCB printing companies will print you 1.6mm. (Some offer 0.8mm)

I figure a 1.6mm would damage the snes cardedge connector, while the 0.8mm would make an unreliable connection. Do you know of any companies willing to print 1.2mm boards, at a fair price?

I've found makepcb.com will print them, but I feel that company is sketchy and has had accuracy problems. (Plus reported 8-10 week delivery time)
I've also found apcircuits.com however they seem to charge a heavy premium for 1.2mm boards. (Upwards of 400 bucks)

Does anyone know of others?

Thanks!

Matt

Yes, you are correct that the proper thickness is 1.2mm (I just measured one to confirm). Check out iTead Studios, they offer a 2-layer 10cmx10cm board for $22, no extra charge for 1.2mm thickness (thicknesses <1.0mm are reasonably cheap) http://imall.iteadstudio.com/open-pcb/p ... 18002.html

Also, if you're interested, I have a PCB outline in EAGLE for all 3 of the standard board shapes (the tiny, no-RAM boards, the standard board, and the large board with the expansion wings). I had to shave the edges down ~1mm on each side to fit within the 10cm size requirement, but they should still fit snug. If you're interested, let me know.

I am interested in the eagle outlines, I have quite a bit of prep work for the schematic of some carts, and the outlines would help get a jumpstart on an open source cart layout.

That is assuming that you are willing to give away your outlines in an open source project.

Yeah, I'm fine open sourcing my library. It's a bit of a mess at the moment, so give me a bit to clean things up a little and I'll send it your way. I'd prefer if you didn't publish the library (mostly because it's a work in progress right now), but schematics can be published without including the libraries without any issues (the only thing is that anyone who downloads the schematic without the library can't edit the footprints). If somebody asks you for the library, I'm fine with you giving it out, I would just rather it not get posted publicly for the time being (again, only due to the current WIP status, I plan to publish it myself eventually).

Wow, this PCB service is actually the cheapest I've seen! They should work perfectly! They even provide Eagle DRC rules which will make my life far easier.

Qwertymodo, I'll keep my eyes on this thread for EAGLE libraries if you would like to post your work. So far I've been using the library for SD2SNES which I pulled out of their GIT. Yours sounds like it would work better given you have explicitly designed it to fit the 10cm requirement.

Thanks a lot for this info!

The downside of batch PCB services like iTead is the long lead time. It easily takes a month to 6 weeks minimum before you get your order back. But their quality is excellent. Even though they allow traces down to 6mil, I'd suggest staying at 10 or greater. Also, I emailed them and they said that they are capable of producing "gold fingers" (the fabrication name for cart edge connectors), so you're good there. Also, depending on the features you need, check out FusionPCB SeeedStudio as well. I believe they use the same fab house as iTead (meaning same quality), but they offer different price breakdowns for different features. http://www.seeedstudio.com/depot/fusion ... p-835.html

Hey Qwertmodo,

Are you still willing to put up your Eagle libraries for SNES cart PCBs? I have picked up a SA-1 PCB (bought PGA Tour 96 for basically nothing at the flea market) and I figure it is a good board to try to replicate. It is fairly square, not too odd of a shape and looks like it could be made to fit the 10x10 cm iTead limit, and the 4" x 3" limit of the Eagle free edition. Plus, has the expansion wings. Ideally I'd like to be able to print a board that will fit inside a real cart. If this is one of the boards you have a design for that would be super, otherwise I am still interested in what you have. I could possibly hit up the flea market again looking for another dirt cheap game to fit it inside. Worst case the cart case can have a date with a dremel and superglue, or even worse case, it could be a board with no case sticking out of the SNES cart slot hehe.

Anyways, let me know! Thanks!

I have a board outline for the carts with expansion wings as well, trimmed a bit to fit within the 10cm width (the original carts are 102mm, not a huge deal, the fitting slots are still there). I have outlines for the No-RAM boards, the normal-sized boards without wings, and the full-sized boards with wings. I don't have any footprints for any of the special chips, so you're on your own there. I do, however, have footprints for the D411, MAD-1, SRAM (narrow and wide, plus the narrow/wide combo footprint you see on most boards), Mask ROM (32/36pin), plus I have footprints for the SuperCIC (DIP and surface-mount) and AM29F032B. Yes, I'm willing to share, but for now just PM me. At some point, when I feel it's more complete, I will likely post it publicly, but for now I've just been handing it out in PM's.

I've updated your library with some changes:

* Set the numbers in the "gold fingers" to Top and Bottom layer, so you can read properly the numbers when hiding one of the layers.

* Added a 42-pin footprint for M27C322.

*Added new footprint for small profile SRAMs (those narrower than usual).

* Added 74LS138, 74LS139 and 74HC257 devices to the library.

If you are interested in taking a look to these changes, please tell.

That was intentional, silkscreen on the bottom layer is supposed to be mirrored. You shouldn't put bottom-layer labels on the top layer and vice versa.


EPROM footprints are always good to have. I really want to get a 3.3v FlashROM working so I can use current-gen, in-production parts, rather than relying on old EPROMS and discontinued 29F032's. Specifically, I'm looking at Micron parts as being a good candidate. They have x8/x16 FlashROMs in TSOP packages up to 1Gbit. Any higher than that and you have to go FBGA.


Those are already in there, though I chose to go the official route and have the dual pinout (the wide pinout with the row of pins in the middle for narrow chips.


Nice, those will be useful.


Sure, I'd be glad to take a look, and probably add some of the new chips. I definitely won't be keeping the pin number silkscreen changes though.

I un-did the changes on this because it caused troubles with iTEADStudio DRU rules. I reverted the "gold finger" pin numbers to your originals.

Please provide any email address so I can send the new library back to you.

my username at yahoo

Since I have the GSU-1 and GSU-2's complete pin-out, I decided to update the Eagle library adding the SuperFX. I have the proper package width and height measured directly on the PCB, but I find hard to get the exact pin distance... Anyone knows? Maybe it is an standard TQFP112?

I have calipers. If I remember, I can measure it. It's definitely not a standard QFP-112, since there are 30 pins on one side and 26 on the other. QFP-112 is square. However, I have a feeling that the pitch is probably the same (0.65mm). Also, note that according to the silkscreen, pin 112 is actually where you'd expect pin 1 to be (so you might check that your pinout accounts for this as well...), so as you count around the chip, you have 112,1...29|30...55|56...85|86...111, and the corner dot is actually at the corner of pin 85|86... which is weird. I haven't actually measured it with calipers, but you can always print out the footprint and see how it looks once you're done. With that many pins, it would be pretty obvious if you were off by even .125mm (which would be the closest standard pitch).

I can't find a GSU to measure, but I do have a Star Fox handy, so here's the MARIO chip. I assume that the pitch is the same for the GSU's.

Thanks!

I'll check when I get my SMW2 back to be sure both are the same pitch. I should use the calipers from my job place.

As for the pin numbering, I didn't get what you said. My board is

http://www.snescentral.com/pcbboards.php?chip=SHVC-1CB5B-01

The pin numbering is the natural one: from 1 to 28 on the left (pin 1 in the dot corner as expected), 29 to 56 on the bottom, 57 to 84 on the left and 85 to 112 on the top side.
Anyway, I did my own checkings to get each pin usage, so even if numbering was wrong, the chip still would work properly.

I'll keep you updated with progress.

Weird... there are apparently 2 different GSU-2 footprints. That seems very odd to me considering they only ever used the chip in, what, 4 games?

http://www.snescentral.com/pcbboards.ph ... C-1CB5B-01
http://www.snescentral.com/pcbboards.ph ... C-1CB5B-20

The second one is the one I was referring to with the odd pin numbering. The first one might actually be a standard QFP-112.

Oh, I see... It's pretty weird...

I think we should continue talking about SuperFX here.

Hey, to anyone who is using my library, magno just informed me I screwed up the board outline. I'm trying to get it sorted out. Also, if anybody who has made additions to my library could send me their updated version, I'll merge any additions along with the outline adjustment and put out an update. This is why I didn't want to release publicly... sorry magno

Hey, no problem, man !!! I send to production as a first step to tune-up the whole process: I deal with PCB boards everyday at work and first prototypes never are as expected. So don't worry about it, I was really convinced that it wasn't going to work in fact.

The best part is that PCB can be inserted by sanding the borders down a bit and pulling out the taps on the upper part of the cartridge, so I finally managed to put it into the enclosure.

I must go now, but I'll send you some photos tomorrow.

I think I see what I did. I initially made the board the same dimensions as an original board, then I shaved it down to fit it within 10cm and in the process I completely got rid of the notches in the top corners on the expansion board, probably intending to take off the entire top 2mm of the board as well, but I didn't. I think I'll go with adding the notches back rather than cutting down the height, the notches give an extra point of contact for holding the board solidly in place. The rest of the issues probably just come down to manufacturing tolerances, so I should probably widen out all of the notches just a bit.

Also, can you comment as to the accuracy of the placement of the circle in the middle of the board with relation to the plastic posts in the cart shell? It's not supposed to be a drilled hole, just a "keep out" region, because the posts press right up against the PCB and any components placed there would make you unable to close the cart. I should probably add that circle to the keepout layers as well, so that the DRC will enforce it (actually, I should add keepout layers to all of my libraries... I haven't been doing that).

Ok, I updated my board outlines. I had the wrong card edge pitch (I was using 2.54mm, it's actually 2.50mm), which I've fixed, and I added in manufacturing tolerances to the outline so there shouldn't be any more issues with the notches being too tight. I also mitered the card edge and beefed up the pin number font (the font size/ratio I was using looked pretty puny and rubbed off a lot on the last batch of boards I ordered).

Oh, I see I also updated the library with my own measures so it would be very interesting to compare. Will you please send it to my email? As for the central circle, I deleted it since it was not actually a hole, only a silkscreen circle and I thought it served not purpouse. Since my board was full of components, I decided to remove it to have more free room to place them.

BTW, it sounds pretty interesting to me what you adviced me: to print the board in a sheet before production. How do you do it to ensure the printed board has the proper size? Do you export it with EAGLE? Do you use some special program to print it?

To print out the board, in Eagle go to File->Export->Image, select a decent DPI (I use 600), then print the resulting image with a photo program capable of printing at the original size, using DPI to specify the size. I use Irfanview. Also, if you place components inside where that circle was, you'll end up having to Dremel down the circular posts in the center of the cart shell, which are designed to stabilize the cart.

Hey qwerty, sent you a pm about these Eagle schematics. Does anyone on here still have them? I'm trying to get some boards made up for testing, but I'm new to working with CAD files so if anyone has those templates that could really help me out!

I'm here for the Eagle library

Meh, what the heck, the link shouldn't chage even if I update the file. Easier to just post it than keep sending it in PM:

https://drive.google.com/uc?export=down ... 0ppalVCN0E

Also, ikari hosts his Eagle libraries for the SD2SNES here so they may be helpful as well