Custom Teensy 3.6 Problems

Status
Not open for further replies.

TomV

Member
Hi,

Ive been trying to build a custom Teensy 3.6, however it is non responsive. The 3.3V supply generated seems good. When pressing the program button I can see both the reset and program signal lines being pulled low.

Attached is the schematic my board uses, I know it's not drawn the best, but if someone could check it over for any obvious mistakes that would be great. When plugging into a PC the first time it makes the sound of a recognised USB device, then after pressing program it never seems to make any sound again. I've built a couple of the PCBs to try and narrow down any bad solder work. Any further troubleshooting suggestions would be great. Thanks.

I've used the following crystal:

EPSON 16MHz Crystal Unit ±10ppm TSX-3225 4-Pin 3.2 x 2.5 x 0.6mm

Screenshot 2019-12-10 at 10.52.20.jpg
 
I'd post all of the related files (now and then again when it's working - to help others). Nothing obvious to me. Use a known good, simple as possible program (eg, blinks LED). Make sure D+/D- didn't get reversed.
 
You do have some other traces running under your crystal trace. How important is it that USB lines be the same length (or maybe they are)? I believe in decoupling capacitors as tight as possible, each one with its own GND via.

Is the MK66FX1M0VLQ18-Teensy symbol available somewhere?
 
You do have some other traces running under your crystal trace. How important is it that USB lines be the same length (or maybe they are)? I believe in decoupling capacitors as tight as possible, each one with its own GND via.

Is the MK66FX1M0VLQ18-Teensy symbol available somewhere?

Thanks for the suggestions. Here's a link to the library used for the MK66, I went through the data sheet to check the pins against this and couldn't see any mistakes. I think I'll make a revision to the pcb to move the traces under the crystal, check the usb length and add decoupling to the MKL04 and see if that works.

https://www.dropbox.com/s/12tmwuryau81s8q/KiCad-Teensy-Lib-master.zip?dl=0
 
The culprit?

Screen Shot 2019-12-11 at 00.07.07.png

Lower the clearance value in the Copper Zone Properties.
Nothing that can't be fixed with a piece of wire and some solder fumes.

Don't know if it is intentional or not but pin13-PTC5(led) is not brought out to any connector.
 
The culprit?

View attachment 18418

Lower the clearance value in the Copper Zone Properties.
Nothing that can't be fixed with a piece of wire and some solder fumes.

Don't know if it is intentional or not but pin13-PTC5(led) is not brought out to any connector.

The pin13-PTC5 is intentionally not bought out, this board is purely to test a custom build. Strangely on my KiCAD it doesn't show a disconnect on the GND plane at that point.Screenshot 2019-12-11 at 11.53.52.jpg
 
Strangely on my KiCAD it doesn't show a disconnect on the GND plane at that point.
There is a "show/hide board ratsnest" button in the left toolbar.
The bottom left statusbar clearly shows "unrouted 1".
Performing a Design Rule Check will also reveal unconnected items.

Screen Shot 2019-12-11 at 14.03.05.png
Screen Shot 2019-12-11 at 14.04.07.png
 
Hope you'll confirm whether or not soldering a wire between those 2 points makes your board work. That sort of feedback can really help everyone else in the future when they're struggling to diagnose a custom board.
 
In my Kicad, those points are connected (through the pin 6 area) and it passes DRC. But you could check the gerbers to verify. Do add more ground vias - think small loops and short, low impedance connections, not just connections.
 
I See it connected the same way as jonr with no errors in the DRC, plus can verify continuity on a PCB here. I'll add more GND vias, move the traces around the crystal, add decoupling to the MKL04 and then re-upload the project here so perhaps you guys can take a look before I send the boards to fab.
 
@jonr
Yes indeed, those points are connected through pin6.

Now if I move that ground plane via 1mil(0.0254mm) up, it then passes DRC.
I suspect there might be some difference between Kicad versions, or different rounding errors depending on the OS used running Kicad.

So my apologies for raising a false alarm.
My setup is MacOS 10.13.6 Kicad 5.1.0
 
It's better, but I'd adopt a general rule that you always put a via to ground as close as possible to every decoupling capacitor (see C9). And every separate Vdd pin has a nearby (as in trace distance) decoupling capacitor (see pin 16). Maybe extend the isolated ground plane under the crystal to also be under the traces.
 
Hi All,

So after being stuck in other projects for the last month or so, I've finally got round to building another test board with a revised PCB to include the changes mentioned above:

Move traces under crystal Traces
Added Vias in more places between Gnd Planes
Reduced the separation distance on Gnd Plane to get more fill
Added decoupling to MKL04


I can report that the board is working! The blink sketch uploaded successfully! Thanks for all the advice to get this going.


T3.6 Test.jpg
 
Status
Not open for further replies.
Back
Top