atmega32u4 schematic and layout feedback

Discussion in 'The Projects Forum' started by bigclick_dean, Aug 9, 2012.

  1. bigclick_dean

    Thread Starter Member

    Jan 24, 2010
    38
    0
    Hi Everyone,

    Just wondering if I could get some feedback on a project I am working on.

    I am building a small arudino based board with the atmega32u4 at the heart, The attached brd and sch files are my first step of getting the basic platform done and then I will customise for each specific task.

    If I could get any tips or feedback on the schematic (including component choice) and the overall board layout that would be great.

    Cheers,
    Dean
     
    • sch.pdf
      File size:
      161.6 KB
      Views:
      43
    • brd.png
      brd.png
      File size:
      46.2 KB
      Views:
      87
  2. bigclick_dean

    Thread Starter Member

    Jan 24, 2010
    38
    0
    Forgot to mention that there is a GND plane on the top I just left it off for this.

    Cheers,
    Dean
     
  3. MrChips

    Moderator

    Oct 2, 2009
    12,415
    3,354
    Three of those blue traces need not be on the bottom layer. Move them to the top layer.
     
  4. bigclick_dean

    Thread Starter Member

    Jan 24, 2010
    38
    0
    Hi MrChips,

    Thanks for taking the time to help!

    Are you referring to the three on the lower right hand side (two data lines and one 5v line)? I have routed those underneath to open up the remaining MCU pins along the two bottom sides so I can route them if needed along the top side. I may also move the via that is just right of the R2 resistor to the left a little to give more routing space for the pins along there.

    Is there a problem with routing the lines along the bottom even if I didn't need that space? Or is it more of a "Why cause more potential problems when you can put them on top in one line of copper"?

    Cheers,
    Dean
     
  5. nerdegutta

    Moderator

    Dec 15, 2009
    2,515
    784
    Hi.

    How about a capacitor on the MCU powerpin to GND? 0.1uF ceramic? How did you calculate R3?

    R = V / I
    R = (5-3.2)/0.02 *
    R = 90Ohm

    * using typical values, as no values for the LED is specified, other than it's RED.

    You do also have an air wire, but I'm sure you know.
     
  6. bigclick_dean

    Thread Starter Member

    Jan 24, 2010
    38
    0
    Thanks for the feedback.

    Which pin are you referring to? I thought I covered most of the power pins with 0.1uf caps and the additional one straight out of the USB port.

    R3 I just grabbed a commonly available (read cheap) resistor as it is only an indicator LED. Is there a problem with doing this? Almost all arduino circuits I have seen have used 1k.

    The led I am using has a Vf of 2v @ 20mA so a 150ohm would be optimal but means I have to order another part ;-)

    I noticed a couple of air wires for the GND that route weird, but I also just noticed the ucap one that goes to C4, is that the one you meant? If so thanks for picking that one up, must have deleted accidentally.

    Cheers,
    Dean
     
  7. nerdegutta

    Moderator

    Dec 15, 2009
    2,515
    784
    Yes, you have, I didn't notice that on the board layout.
    I guess the only thing is that the LED will be dimmer...
     
  8. MrChips

    Moderator

    Oct 2, 2009
    12,415
    3,354
    Yes, no point in making life more difficult than you have to.
    Same reason for not running traces in between IC pins.
     
  9. bigclick_dean

    Thread Starter Member

    Jan 24, 2010
    38
    0
    Sweet, does that mean my decoupling is a pass? ;-) being that it is relatively low frequency use I cannot see any issues.

    Dim LED should be fine, it will more than likely be left out of the final production board anyway as it will end up in an enclosure, just like it when prototyping so I can see where I break stuff!

    Cheers,
    Dean
     
  10. bigclick_dean

    Thread Starter Member

    Jan 24, 2010
    38
    0
    Thanks for the clarification, makes sense as vias just add another point of failure and if you don't need to do it then why do it.

    As I will be using this design for a couple of different end products would I be best to keep them all the same even if I could route some along the top simply for a consistency point of view? Or route every board as efficiently as possible with no consistency?

    Cheers
     
  11. MrChips

    Moderator

    Oct 2, 2009
    12,415
    3,354
    Low or high frequencies, you still need power supply decoupling capacitors.

    All your capacitors and LED are not connected to the ground plane. Same for all GND connections.

    Any particular reason for choosing that orientation of the MCU chip. I would have turned it 180 degrees. You want to keep the USB D+ and D- traces short and symmetrical.
     
    Last edited: Aug 10, 2012
  12. t06afre

    AAC Fanatic!

    May 11, 2009
    5,939
    1,222
    As I see it the reset input is left floating then reset not activated. In general a very bad design approach:eek:. The reset pin may have a internal pull-up resistor. But these are ofyen quite large like 100K. This is a common and simple way of doing it
    [​IMG]
    The question is do you really need a rest button in this application at all.The way you have have drawn the decoupling caps are OK. But some text explaining the use of these caps. In the schematic, could helped a lot
     
  13. bigclick_dean

    Thread Starter Member

    Jan 24, 2010
    38
    0
    Thanks again for your input, I understand the need for the decoupling caps but I was more referring to the distance from the 5v lines and general layout/component selection.

    I have a GND plane on the top side that connects all of the GNDs but left it off for ease of reading.

    There was no real reason behind the orientation, rotating it around 180 to get the D+- to the left hand side is a great idea, I will give it a go and upload a revised version to see if it causes any other issues (shouldn't do though as it is a pretty basic circuit with low component count).

    How symmetrical do the D+- lines have to be? are we talking down to a couple of mm or is there a bit more room to move there. As an idea of speeds required, they are connecting at low speed serial.

    Regards,
    Dean
     
  14. bigclick_dean

    Thread Starter Member

    Jan 24, 2010
    38
    0
    Thanks for that, I had the same questions going around my head about the reset button and if it was actually required. For the dev boards I will have it just for ease of use but it may also be required for firmware upgrades to initiate the bootloader. I am going to be checking out the USB reset feature and see if that will work instead and then dropping the reset button from the final design.

    There is an internal pull-up for the reset line but I couldn't find a reference the the value from a quick scan of the datasheet. What value for R1 would you suggest in your circuit? If I was to drop the button all together would you still suggest connecting it to 5v with a resistor or just leave it floating? Would leaving it floating leave it open to potential random resets in a high noise environment? For the sake of a 2c resistor....

    Schematic feedback is appreciated also, when I am rotating the MCU I will tidy up the schematic diagram a bit with some more info and put it back up again.

    Cheers,
    Dean
     
  15. MrChips

    Moderator

    Oct 2, 2009
    12,415
    3,354
    What CAD software are you using?
     
  16. MrChips

    Moderator

    Oct 2, 2009
    12,415
    3,354
  17. bigclick_dean

    Thread Starter Member

    Jan 24, 2010
    38
    0
    I am using eagle at the moment as I am on a mac, I like Dip Trace also but the mac version (wine wrapper) is pretty buggy and the current version doesn't have great eagle importing for parts I need.

    Thanks for the guidelines, are those general or ATMEGA specific ones, I am pretty sure I used something similar to that to design the schematic.

    I will flip the chip and see how much shorter I can get the data lines.

    Cheers,
    Dean
     
  18. bigclick_dean

    Thread Starter Member

    Jan 24, 2010
    38
    0
    So I have taken the feedback on board and here is my 2nd attempt, the IC1 has been rotated 180° to shorten the data line length and I have also added an additional LED for the PE6 line (for debugging).

    I have upped one of the decoupling caps to 10μF from the 1μF one I had and left the other 3 at 0.1μF

    Air wires fixed and a general rearrange.

    Any suggestions appreciated.

    Cheers,
    Dean
     
  19. nerdegutta

    Moderator

    Dec 15, 2009
    2,515
    784
    Looks better.

    Have you checked the connections to C1 on the board? Look too me like there only one pin on the capacitor that is connected...
     
  20. bertus

    Administrator

    Apr 5, 2008
    15,638
    2,344
    Hello,

    It looks like that the right side of the Xtal is grounded.
    I think that you should make that side free and shift C1 accross the opened space.

    Bertus
     
Loading...