Forum Discussion
Altera_Forum
Honored Contributor
Honored ContributorMax10 PCB Layout - Unused Pins
Hello,
I am building my first from-scratch FPGA project. I’m using a Max10 10M02SC 153-MBGA, but my design is really simple. I really only need to use one bank because I only need about 16 I/Os. (I started with a smaller Max10, but I wanted the single-supply option to keep my PCB simpler.) I’m running everything at 3.3V, and I’m not using the ADC or anything else fancy. I don’t even have an external clock- I’m using the Max10’s built-in clock. I’ve tested the design on an evaluation board, and it does work. So, I am now going to have around 100 unused pins. I have read many places that I can set them to “inputs tri-stated with weak pull up” and then I don’t need to even connect them to the PCB. Is that correct? My big reason for asking is this: because my design is so simple, and low-speed (external clock speeds are about 14kHz), I would like to eliminate some of the MBGA pads to allow easier trace routing to other pads. This way I can keep the PCB to 2 layers and hopefully not need expensive laser-drilled microvias. Does this sound reasonable? I do intend to connect all of the VCCIO, VCC_ONE, VCCA, and GND pins, so there will still be a lot of mechanical stability. Thanks!13 Replies
Altera_ForumAny unused pin should be connected to PCB as a pad which doesn't route any where. This helps during assembly.
About the MAX10's clock, you might want to consider placing spare clock source as backup. MAX10's internal clock has big range of uncertainty. If your design doesn't care "exact time", then you will be okay. Another recommendation is to bring out test points on unused pins for debugging or for spare. It's just a practice. Lastly, review PCG-01018 document which is max10 fpga device family pin connection guidelines. Regards, Kevin- Altera_Forum
Hi Alex,
Thank you very much. That's good info, which is what I need! OK, since I have never routed a BGA before, I was looking at Altera's document on how to do it (an114 (https://www.altera.com/content/dam/altera-www/global/en_us/pdfs/literature/an/an114.pdf)). They seem to indicate that you must use in-pad vias, and, since the pads are so small, this means you must use microvias. So how did you route this package without the microvias? Any tips you can give me wold be greatly appreciated! Thanks again! Robert - Altera_Forum--- Quote Start --- I can set them to “inputs tri-stated with weak pull up” and then I don’t need to even connect them to the PCB. Is that correct? --- Quote End --- In this instance they need not be electrically connected. You're correct in that regard. However... If I understand your post correctly you're proposing to remove PCB pads for device pads that are not used. Correct? In theory this is fine. However, I would anticipate you having difficulties assembling this. Without an associated pad for the MBGA ball to reflow to, I'd anticipate problems. What will this reflowed solder ball (from the package) do without a pad? Will it behave and solidify in situe or, without the expected reflow shape, will it end up shorting to another pin? You may well find this is not an issue. Dropping a pad or two certainly wouldn't be an issue for traditional 'legged' devices and I suspect with larger pitch BGA devices you could well get away with this. Even if your unused input with pull-up does short to another pin - so what? As long as it only shorts to one other pin. --- Quote Start --- keep the PCB to 2 layers and hopefully not need expensive laser-drilled microvias --- Quote End --- I strongly recommend you look to 4 layers for such a device. I've routed this package (although not MAX 10), on 6 layers, without the need for any micro-vias. You should be able to find a standard PCB technology that allows you to do all you need without the need to remove any pads. Cheers, Alex
