Forum Rule: Always post complete source code & details to reproduce any issue!
Results 1 to 21 of 21

Thread: Custom Teensy 3.6 Problems

  1. #1
    Junior Member
    Join Date
    Dec 2018
    Posts
    11

    Custom Teensy 3.6 Problems

    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

    Click image for larger version. 

Name:	Screenshot 2019-12-10 at 10.52.20.jpg 
Views:	38 
Size:	115.3 KB 
ID:	18407

  2. #2
    Senior Member PaulStoffregen's Avatar
    Join Date
    Nov 2012
    Posts
    21,354
    Can't read the schematic. Maybe a PDF would be better?

  3. #3
    Junior Member
    Join Date
    Dec 2018
    Posts
    11
    Custom3.6Driver.pdf

    Hi Paul.

    Should be attached now, hopefully this is clearer. Thanks.

  4. #4
    Senior Member
    Join Date
    May 2015
    Location
    USA
    Posts
    329
    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.

  5. #5
    Senior Member PaulStoffregen's Avatar
    Join Date
    Nov 2012
    Posts
    21,354
    Schematic looks like it ought to work.

    Maybe something wrong in the layout? Here's a project where the schematic was perfect, but the problem turned out to be a missing trace in the layout. It can happen....

    https://forum.pjrc.com/threads/41994...751#post134751

  6. #6
    Junior Member
    Join Date
    Dec 2018
    Posts
    11
    Heres a link to a Kicad project if you have chance to glance over that at all. I can't see anything obvious in the layout.

    https://www.dropbox.com/s/j8ysvsdnly...Files.zip?dl=0

  7. #7
    Senior Member
    Join Date
    May 2015
    Location
    USA
    Posts
    329
    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?

  8. #8
    Senior Member
    Join Date
    May 2015
    Location
    USA
    Posts
    329
    Also, the MKL04 doesn't have a decoupling capacitor anywhere close.

  9. #9
    Junior Member
    Join Date
    Dec 2018
    Posts
    11
    Quote Originally Posted by jonr View Post
    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/12tmwuryau...aster.zip?dl=0

  10. #10
    Senior Member
    Join Date
    Nov 2017
    Location
    Belgium
    Posts
    215
    The culprit?

    Click image for larger version. 

Name:	Screen Shot 2019-12-11 at 00.07.07.png 
Views:	13 
Size:	77.1 KB 
ID:	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.

  11. #11
    Junior Member
    Join Date
    Dec 2018
    Posts
    11
    Quote Originally Posted by neurofun View Post
    The culprit?

    Click image for larger version. 

Name:	Screen Shot 2019-12-11 at 00.07.07.png 
Views:	13 
Size:	77.1 KB 
ID:	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.Click image for larger version. 

Name:	Screenshot 2019-12-11 at 11.53.52.jpg 
Views:	6 
Size:	121.2 KB 
ID:	18422

  12. #12
    Senior Member
    Join Date
    Nov 2017
    Location
    Belgium
    Posts
    215
    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.

    Click image for larger version. 

Name:	Screen Shot 2019-12-11 at 14.03.05.png 
Views:	1 
Size:	18.5 KB 
ID:	18423
    Click image for larger version. 

Name:	Screen Shot 2019-12-11 at 14.04.07.png 
Views:	3 
Size:	105.8 KB 
ID:	18424

  13. #13
    Senior Member PaulStoffregen's Avatar
    Join Date
    Nov 2012
    Posts
    21,354
    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.

  14. #14
    Senior Member
    Join Date
    May 2015
    Location
    USA
    Posts
    329
    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.

  15. #15
    Junior Member
    Join Date
    Dec 2018
    Posts
    11
    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.

  16. #16
    Senior Member
    Join Date
    Nov 2017
    Location
    Belgium
    Posts
    215
    @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

  17. #17
    Junior Member
    Join Date
    Dec 2018
    Posts
    11
    Im Running OSX 10.14.5, And Kicad 5.1.4. Here are some updated files if anyone has a chance to glance over them for silly mistakes before I send to fab.

    Changes Include:

    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


    https://www.dropbox.com/s/zf30zadw5p...0V1.1.zip?dl=0

  18. #18
    Senior Member
    Join Date
    Nov 2017
    Location
    Belgium
    Posts
    215
    Pcb looks good at first glance. DRC ok.
    My setup is MacOS 10.13.6 Kicad 5.1.0
    correction: Kicad 5.1.5

  19. #19
    Senior Member
    Join Date
    May 2015
    Location
    USA
    Posts
    329
    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.

  20. #20
    Senior Member crees's Avatar
    Join Date
    Dec 2016
    Location
    Utah
    Posts
    210
    TOMv Can you take a clear picture of the board with all the pins of the K66?

  21. #21
    Junior Member
    Join Date
    Dec 2018
    Posts
    11
    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.


    Click image for larger version. 

Name:	T3.6 Test.jpg 
Views:	7 
Size:	110.3 KB 
ID:	18850

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •