Hello, I’ve got a fairly complicated and dense PCB I want to clarify the layout on before i move to finalizing the silkscreen. About the board:
- It's a micro-quadcopter control board, measuring 1.5" square to save weight and stretch the limits
- I plan to have these fabbed by SeeedStudio; they offer 6 mil trace/space and 12 mil vias, 0.8mm thick PCB to save weight
- Components onboard: HMC5883L magneto, BMP085 barometer, MPU6050 accel/gyro, Copernicus II GPS and chip antenna, TPS61200 boost converter
- Central chip is a PIC32MX795F512H
- Headers broken out include 17 GPIO, programming header, serial port, USB port, and 5 PWM control lines
- At any one time, no more than 120ma is expected from the TPS61200
Clockwise from upper left: TPS61200, HMC5883L, BMP085, MPU-6050, GPS antenna, PIC32 in the center, and Copernicus II underneath. Longest continuous headers on the left and bottom are GPIO, top 3x5 headers are servo ouptputs, the 2-pin header is battery input, the 5 pin header is for programming, the top 4 pin header is a serial port, and the bottom 4 pin header is a USB port.
I will include ground planes top and bottom but am not sure how to “remove” copper underneath the magnetometer in the upper right corner.
Any feedback is greatly appreciated, I’m only 14 and eager to learn.
looks fine, though It it looks like you could make the tracks same width as the pads on the pic without any big problems, no need to go to the limit if you don’t have to.
I would put a via in the center pad of the TPS61200, that way you can solder it by hand from the backside and it’ll get a bit more cooling connected to the ground plane one the back as well
drawing a rectangle on the bRestrict layer should remove copper from the plane on the bottom side
I’d make the connections between pads (both th and smt) and planes with thermals, otherwise you will have a very hard time soldering them.
Are you allowed to have any copper under the antenna? Also, check the underside of your batterty holder for exposed metal that could short out to the vias; not sure if that’s a problem with the one you have chosen.
As above, your pads that are connected to the plane are completely surrounded and will make for hard soldering - more likely to damage the component. Use thermal relief.
Where the tracks exit the headers - thicken them as much as you can. the board is going to be subject to shock when the copter crashes and connectors/wiring may cause the junction to flex and break on such thin tracks, make them thicker while it exits and there is less chance of that.
What clearance between the planes and tracks have you got?
Have you run a DRC check?
Such a fine copper to copper gap puts the cost of the board up.
Ditto about copper under the antenna. You should also not run tracks under it - move it to where the “Microquad V2” text is away from other tracks and features.
On the underside there are 3 vertical tracks in the middle of the board, route them to the left a bit more and reflood and you will get a better plane connection through. bottom side IC, 3rd pin bottom left - mitre the track more to allow a better ground through.
I researched the antenna problem and rerouted the traces, as well as add some vias between the top and bottom planes. I adjusted some traces, checked the DRC, and everything works fine. I decided not to add thermals since I’ve never had a problem at all with soldering without them on my first version of this board, and it looks nicer in my opinion. The traces leading up to the headers won’t be under and stress really since the copter is so small (<40g, 5" across) that it’s actually hard to break when crashing.
Here is a web page that will help you decide what you need for minimum circuit board trace widths. You tell it how much power you’re moving through the traces and how thick the traces are, and it will calculate how wide to make your traces. “Thickness” refers to how many ounces of copper per square foot of board size. Typically, board houses use 1 oz copper per square foot. If you need more power but don’t have room for wider traces, go to 1.5oz or 2 oz copper. The cost is not that much higher.
What exactly is wrong with the layout? I kept the components close and followed the recommended components on the datasheet. I kept traces short and more than sufficient to handle the current. Is the grounding for power and control the issue?
Your components aren’t close enough; specifically, ground connections of input and output capacitors are too far away from the controller. Also, inductor is too far from the switch node. Switcher layout is complex - I gave you the link to the good layout, study it. You may also want to look at the layout of TPS61200 evaluation board, it is also good if output capacitor package is not large enough to run AUX capacitor trace underneath it.
It is possible that your design will work without issues, in this case nothing needs to be done. My suggestions are given in case you will have issues with the supply.
