Forum Rule: Always post complete source code & details to reproduce any issue!
Results 1 to 22 of 22

Thread: Designing my own PCB - assistance

  1. #1

    Designing my own PCB - assistance

    Hello all

    I am having a go at designing my own PCB for a project. My first design uses a standard Teensy 3.2 directly mounted on top of the pcb for ease.

    However, this uses up a lot of real estate, especially as I am not actually using that many of the pins.

    I thought my second attempt would be to try and reproduce a Teensy 3.2 in component form. I found the circuit diagram, but I have questions about a few of the parts/connections.
    But, this is my first attempt, so not really sure what the heck I am doing (but there is only one way to learn).

    https://www.pjrc.com/teensy/schematic.html

    1. Ferrite coils connected to pins 7 and pins 16. What value? I guessed 120R?
    2. Resistors that are unmarked (470? attached to pin 14, 33? attached to pins 5 & 6). Again, I am assuming these are 470R and 33R.
    3. Diodes on pin 23. What is 1A?
    4. Capacitors. They are shown as having polarity, yet surely these are just small polyester type caps?

    I believe I can eliminate most of the capacitor/ferrite suppression that feeds AGND, as I am not using any analogue inputs (therefore not using AGND).

    Anything else I should be aware of? (Apart from the chances of it working first time are slim!). The Crystal. I understand this needs to be surrounded by a ground plane?

    I can imagine the eyes rolling as I type

  2. #2
    Senior Member
    Join Date
    Jul 2020
    Posts
    472
    Quote Originally Posted by SteveSFX View Post
    Hello all

    I am having a go at designing my own PCB for a project. My first design uses a standard Teensy 3.2 directly mounted on top of the pcb for ease.

    However, this uses up a lot of real estate, especially as I am not actually using that many of the pins.
    Really? You are allowed to populate the region of your pcb between the header rows, so you only lose those
    rows of connectors, and if you use surface-mount connectors you only lose pcb area on one side, and if
    using through-hole you only need the header pins you use, plus one at each corner perhaps.

    I thought my second attempt would be to try and reproduce a Teensy 3.2 in component form. I found the circuit diagram, but I have questions about a few of the parts/connections.
    But, this is my first attempt, so not really sure what the heck I am doing (but there is only one way to learn).

    https://www.pjrc.com/teensy/schematic.html

    1. Ferrite coils connected to pins 7 and pins 16. What value? I guessed 120R?
    Inductors won't be in ohms! The other schematics don't say whether nH, ÁH or mH alas, I'd guess ÁH are meant but
    not certain. [The schematic needs fixing with the units added!]
    2. Resistors that are unmarked (470? attached to pin 14, 33? attached to pins 5 & 6). Again, I am assuming these are 470R and 33R.
    Resistor values are in ohms, yes! Those resistors are LED current limiters by the look of it so the values in hundreds of ohms
    are clearly credible. Not sure about the resistors in the other schematics with values in kelvin though(!) - this isn't because
    lower case is unavailable.
    3. Diodes on pin 23. What is 1A?
    1 ampere, though the other boards use BAT54C which is not rated 1A, and is not a pn-junction diode either, its schottky
    (different symbol), although this isn't critical I think.
    4. Capacitors. They are shown as having polarity, yet surely these are just small polyester type caps?
    They are incorrectly shown as polarized, and they are ceramic, not film - clear from the brown colour and tiny size.

    I believe I can eliminate most of the capacitor/ferrite suppression that feeds AGND, as I am not using any analogue inputs (therefore not using AGND).
    You have to connect VSSA and VDDA whether used or not though (just in case you don't know this).

    Anything else I should be aware of? (Apart from the chances of it working first time are slim!). The Crystal. I understand this needs to be surrounded by a ground plane?
    Not really, it should be kept away from current-carrying traces though. The loading caps will couple it capacitively to
    ground anyway, but crystals are often run at low power and thus susceptible to noise pickup. Keep it close to the pins.

    Make sure your decoupling is thorough, the smallest value caps need to be right on the power pins to minimize
    inductance between pin and first cap. All power pins need decoupling, not just some of them (they wouldn't
    bother pinning it out if not required). The use of multiple ground and power pins on a chip is to reduce inductance,
    nothing to do with current handling.

    I can imagine the eyes rolling as I type

  3. #3
    Senior Member
    Join Date
    Jul 2014
    Posts
    2,900
    Quote Originally Posted by MarkT View Post
    Inductors won't be in ohms! The other schematics don't say whether nH, ÁH or mH alas, I'd guess ÁH are meant but
    not certain. [The schematic needs fixing with the units added!]
    The ferrite chip is indeed indicated as 120 Ohm impedance (most likely at 100 Mhz as in most cases)

  4. #4
    Thanks for the advice.

    Oh I TOTALLY realise that I am not going to be anywhere near as efficient as the Teensy board design. It's more of a learning curve thing than anything else.

    I have populated under the Teensy board in my first design.

    I used BAT54 diodes another part of my project, so I will use those.

    When you say decoupling 'right on the pin'. I am about 10mm away in a few cases. OK?

    I don't need the USB socket, as I am wiring a USB A directly into the project.

    So, the Micro USB has 5 pins. 5v, D+, D-, Ov and mode (I assume). Am I correct in thinking that when using a 4 pin USB A lead, the fifth mode pin that goes to the flash IC (MKL02Z32VFG4) pin 6 goes to ground?

    You mention loading caps on the crystal, but I don't see them on the schematic. Should that be a pair of 18 or 22pf caps to ground?

    My VSSA and VDDA are linked with the 2.2uf cap shown in the diagram.

    Well, it's a learning curve!

  5. #5
    Senior Member
    Join Date
    May 2015
    Location
    USA
    Posts
    727

  6. #6
    Senior Member
    Join Date
    Jul 2020
    Posts
    472
    Quote Originally Posted by SteveSFX View Post
    Thanks for the advice.

    Oh I TOTALLY realise that I am not going to be anywhere near as efficient as the Teensy board design. It's more of a learning curve thing than anything else.

    I have populated under the Teensy board in my first design.

    I used BAT54 diodes another part of my project, so I will use those.

    When you say decoupling 'right on the pin'. I am about 10mm away in a few cases. OK?
    Yes, I reckon, but make sure the trace between the pin and cap isn't too skinny and runs over ground-plane
    to keep the inductance low.

    I don't need the USB socket, as I am wiring a USB A directly into the project.

    So, the Micro USB has 5 pins. 5v, D+, D-, Ov and mode (I assume). Am I correct in thinking that when using a 4 pin USB A lead, the fifth mode pin that goes to the flash IC (MKL02Z32VFG4) pin 6 goes to ground?

    You mention loading caps on the crystal, but I don't see them on the schematic. Should that be a pair of 18 or 22pf caps to ground?
    They are probably in the chip itself, I'd check the datasheet section on this, it will indicate suitable specs for the crystal.

    My VSSA and VDDA are linked with the 2.2uf cap shown in the diagram.

    Well, it's a learning curve!

  7. #7
    Senior Member
    Join Date
    Jul 2014
    Posts
    2,900
    Quote Originally Posted by MarkT View Post
    They are probably in the chip itself, I'd check the datasheet section on this, it will indicate suitable specs for the crystal.
    Yes, they are in the chip and can be changed by software. Years ago, FrankB made a sketch that played "FM music" by changing theses capacitors.

  8. #8
    Thanks all

    I actually have managed to make a reasonable first attempt. Stupid things like 'why have 3x 2.2uf caps in a row?' on the schematic become suddenly ... 'derr, one on each pin'.
    My caps are basically on the pins now.

    I added caps for the crystal. I will remove those.

    Track widths? Went with what was standard (and fitted the IC patterns).

    I have NO DOUBT it will have issues, but hey ho.

    This includes an SD card reader as well.

    Click image for larger version. 

Name:	Pic-1s.png 
Views:	20 
Size:	23.9 KB 
ID:	22066

    Click image for larger version. 

Name:	Pic 2.gif 
Views:	17 
Size:	14.8 KB 
ID:	22067

  9. #9
    Senior Member
    Join Date
    May 2015
    Location
    USA
    Posts
    727
    I think your crystal is sharing a line with something else. I wouldn't do that.

  10. #10
    Yes... I spotted that when I removed the 18pf capacitors....

    Although, those 2 shared pads are ground. Should I leave those unconnected or maybe join to the ground plane when I copper pour the spaces on the board? (which I was going to ground)

  11. #11
    Senior Member
    Join Date
    Jul 2014
    Posts
    2,900
    Quote Originally Posted by SteveSFX View Post
    Yes... I spotted that when I removed the 18pf capacitors....

    Although, those 2 shared pads are ground. Should I leave those unconnected or maybe join to the ground plane when I copper pour the spaces on the board? (which I was going to ground)
    There are special considerations concerning ground and connections for Xtal. There were discussed here in the forum. A search may find them.

  12. #12
    Hmm... I have been searching, and found various results.

    I am wondering whether to simply put a pad next to the crystal connected to its dual ground connections, then I can link that across to the ground flood if I wish.

    As I said, I have no doubt this first circuit attempt will have issues.

  13. #13
    Senior Member PaulStoffregen's Avatar
    Join Date
    Nov 2012
    Posts
    23,040
    Quote Originally Posted by SteveSFX View Post
    I am wondering whether to simply put a pad next to the crystal connected to its dual ground connections
    Please read the suggestions for the crystal on the MKL02 page:

    https://www.pjrc.com/store/ic_mkl02.html

    Scroll down to "Crystal Guidelines".

  14. #14
    Senior Member
    Join Date
    May 2015
    Location
    USA
    Posts
    727
    +1 on what Paul said. Since this keeps coming up, here is one that can be copied. Note the guard ring and single ground connection point. Not shown is the continuous ground plane under it. Maybe someone else has a more perfect example.
    Attached Thumbnails Attached Thumbnails Click image for larger version. 

Name:	crystal.png 
Views:	6 
Size:	111.2 KB 
ID:	22071  

  15. #15
    Thanks chaps

    I 'think' I am OK.

    Do you think a ring of ground around the crystal like that helps?

    I have run a 'clean' ground directly from the incoming supply, straight to the crystal. Doesn't share with anything else. Also shortened the leads to the crystal to the minimum distance I could achieve.
    No other traces go under it or near it.

  16. #16
    Senior Member
    Join Date
    May 2015
    Location
    USA
    Posts
    727
    It probably helps (lower jitter?), but experience says it isn't necessary.

  17. #17
    Senior Member PaulStoffregen's Avatar
    Join Date
    Nov 2012
    Posts
    23,040
    Whether the gaurd ring matters really depends on the type of signal which you route close to the crystal. For example, the reset signal doesn't actually change voltage while the chip runs, so it would have little to no impact. Signals from the I/O pins can vary in their impact, most depending on whether the software configured slew rate limiting on that pin. Fast rising & falling edges are the enemy here.

    Physical distance also matters. If you're designing with 8 mil (0.2mm) spacing between traces, the capacitive coupling effect is much less than if your spacing between traces is only 6 or 4 mils (0.15mm or 0.1 mm).

    In theory, you could just keep stuff away from the crystal. But the practical reality of most PCB routing involves a lot of human effort to cram traces through available spaces. Allocating the space for the crystal's guard ring and bottom-side copper fill before you route the rest of the PCB (and leave them intact and consider them "untouchable" while working) tends to be the most realistic approach to end up with a high quality design.

  18. #18
    Thank you for all the advice.

    I am pretty happy with my first go. The crystal is out on it's own, and there are not really many switching lines on this PCB, it's mainly I2C and serial to a couple of other IC's.

    I checked the circuit through earlier against my circuit diagrams. Seems correct, but there is only one way to find out.
    I think I will populate the IC minus the processor, and test the processor pinouts before committing to fitting the main IC.

    Click image for larger version. 

Name:	Pic3.jpg 
Views:	9 
Size:	267.6 KB 
ID:	22080

  19. #19
    Hi

    Just wondered if anyone has a suggestion for a right angled PCB mount (through hole or SMD) connector?

    10 way and ideally needs to project out slightly from the PCB so it can exit the case.

    It is solely used for triggering signals, so negligible load.

    I have designed my PCB using this connector, but they are VERY expensive. However I cannot find a better solution (yet).

    https://uk.rs-online.com/web/p/products/7393942/
    https://uk.rs-online.com/web/p/products/7393762/

    Now these connectors go directly to my TEENSY as trigger inputs. Can someone suggest a way to protect these switch inputs? I was thinking Opto isolators, but not used those before.

    Thanks!

  20. #20
    I found this diagram in this forum... I like the idea of having 5v - 24v input ability. Seem ok?

    Name:  Opto isolator MOCD208 - 5v to 24v.png
Views: 125
Size:  24.2 KB

  21. #21
    Hello all

    Still plodding on with my project. All going OK.

    I assume all these capacitors on the Teensy are SMD ceramic. I am planning to add a couple of larger electrolytic caps to my 3.3v regulator (to help with smoothing). Should not be a problem?

  22. #22
    Hello clever folk

    I have a question regarding capacitors (again).

    My Teensy circuit diagram shows 0.1uf capacitors. We have already deducted that they incorrectly show them as electrolytic.
    I have other circuit diagrams here for other circuits, for instance an SD card controller. This shows 100nf capacitors as suppression. May I ask if there is any difference here at all for these smoothing caps?

    Unless my maths is worse than I thought, 100nf is 0.1uf. Is it purely down to personal choice of what description of the value you use?

    As a standard. I have been placing an SMD 100nf capacitor across the supply of every IC on my PCB, as close to the IC as I can get it. Is that overkill? Can you have too many capacitors across the 3.3v rail?
    Think I now have 12 spaced out across the pcb.

    The 3.3v supply has a 100uf electrolytic on its 5v input, and a 10uf on it's 3.3v output (as the datasheet showed).

    This has proved to be an interesting project. I will update with pics if anyone is interested.

    Thanks

Posting Permissions

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