Hello, I am routing a eMMC chip for a system, and it contains many NC pins that the datasheet explicitly says may be routed through.
Considering the pitch of the BGA and the number of actual (not NC) pins on the eMMC this makes since and seems to be important for good routing since I am trying to keep them mostly on the same layer.
What would be the most elegant way to make it so that you can freely route through the pins without having to connect them in the schematic?
Why would you need to have the NC pins in the schematic? If they’re not there, they have no net and you should be able to route through them freely.
But I admit I’ve never tried it myself.
Best way is to connect these pins in schematic.
It doesn’t work like that.
Just tested it myself. You’re right.
Nasty limitation.
You can do this with “pin stacking” in the schematic symbol. (set the extra pins to passive and then place them on the same location as the real pin.
Another way, (bit of a dirty trick) is to simply remove the pads from the footprint altogether. But then there would be soldermask on that location, and this may lead to production problems. Instead of just deleting the pad, you can also set it to an aperture pad in the footprint editor, and then poke a hole though the solder mask. I verified this and you can indeed just route though an aperture pad.
(Edit: Ah, dammit. I thought for a moment there was something like a free pin type (See scone below), and then got distracted again)
Another way would be to use the “free” pin type, though this requires editing the symbol. The big perk is this removes the need to plan in advance which pads are routed through by which nets.
I ended up not finding this out because I had the pins stacked. So when I first tried this they registered as all interconnected. You must unstack them for this to work. Seems like a reasonable compromise was to unstack them all, then set them as free and not visible.
I apricate this a lot thank you! It will keep the design much more maintainable.
If you hide pins, is usually best to also move them to the inside of the symbol. This reduces the chance of a wire connecting to it in the schematic. I’m not sure what a wire connected to a free pin does in the schematic.
