Electronics > PCB/EDA/CAD

Stuck in PCB routing: where do I go from here?

(1/3) > >>

exscape:
Here's where I'm at:
--- End quote ---


As the finely-drawn arrows indicate, I need to route those pins across the thick 5 V trace that goes through the middle of the microcontroller (the DIP package, U4).
What's the best technique for doing so?
This is on a 2-layer board, where the bottom layer will be a ground plane. Some of the pins are relatively high frequency, 8 MHz SPI. I can lower that frequency if needed, but I prefer to do this properly, over doing it badly and slowing the circuit down until it works.

Routing around isn't an option, as the power trace goes pretty much from top to bottom of the PCB.
My first thought was to use vias for the signal traces, but that'd make 12 of them (if I bring them back to the top layer again)...
My second thought was to move the 5 V trace (the Y-split part) onto the bottom layer, but then I'd be routing the signal traces over a split in the ground plane. Not good for signal integrity/EMI.

This is my first proper PCB layout, by the way, so I'm indeed new to this. :)

8086:
You can drop the 5V trace down and then back up for a short run, shouldn't cause problems.

jeremy:
is there a reason you can't shift the isp to the left hand side and move your reg over ? anyway, unless your design critically depends on a ground plane with exact geometry (at 8Mhz, I assume not), I don't see why dropping a few power tracks down for a little bit should be a problem. Some of the guys I work with would consider 8Mhz to be DC!

Perhaps it would help to know what you are building. Good luck!

HackedFridgeMagnet:
Can you do a surface mount zero ohm link for the 5v and run the tracks between the link? Obviously it would need to be fairly large the gap, or you could do multiple links like this.

I think I would just use the second layer for a short bit of 5v. As the ground plane is already broken by the through hole stuff anyway.

ps. I am no expert at this.

mikeselectricstuff:
Small breaks in a ground plane are not a problem in the vast majority of cases.
The general technique for mostly SMD boards is to do as much as you can on the top layer, and do small jumps via a the bottom layer ground plane where necessary, and when finished space them out or group them together as required to avoid splitting the plane
PCB layout will always be a compromise, and all rules and recocmmendations are flexible.
Things which are critical on PCBs using things like 24 bit ADC or  1GHz+ radios can be completely ignored on most run-of-the-mill PCBs. Also remember that you generally have routing space around the edge on both sideswithout worrying about cutting things off.
The only absolute rule is that good placement is everything!


Navigation

[0] Message Index

[#] Next page

There was an error while thanking
Thanking...
Go to full version
Powered by SMFPacks Advanced Attachments Uploader Mod