Shop OBEX P1 Docs P2 Docs Learn Events
First PCB - Please Check — Parallax Forums

First PCB - Please Check

mhamen3mhamen3 Posts: 69
edited 2011-05-13 07:52 in Propeller 1
Hi guys,

I've designed a board for a project I've been working on http://lynxmotion.net/viewtopic.php?f=8&t=7256. It has an Xbee module in the upper left, 3 I/O Headers (2 for servos run at 7.4V with their own battery terminal and 1 for 4 hall effect sensors to read shaft rpm which can be jumpered to 5v), in the upper middle there are 2 pin outs for TB6612FNG motors drivers. There will be two driver boards stacked on each pin out. I'll be driving 4 motors but will be running the boards in parallel. There's the power supply on the right and the eeprom and prop plug header on the left of the prop.

Please review this; any criticism is welcome. It is still a work in progress and is still kind of crude. This is my first time designing a board and I know there are some things that I must be overlooking.

Thanks,
Marc
HybridQuad Draft1.jpg
HybridQuad Draft1.jpg
1024 x 640 - 123K

Comments

  • LawsonLawson Posts: 870
    edited 2011-05-09 22:18
    A couple things pop out. First the reset switch and "NOT" chip appear to be missing connections. Second, the power jumpers between the servo header blocks look crowded. Third, there are no decoupling capacitors anywhere. The capacitors are small (<1uF) ceramic capacitors placed between the power traces next to high frequency parts. They "stiffen" the power supply locally, because at 80MHz switching frequencies, the inductance of a few inches of trace is significant. (go ahead and hide the capacitors under the DIP parts) Fourth, I'd suggest adding a ground plane to one of the layers. A ground plane simplifies layout and helps a ton with EMI immunity. Fifth, I recommend reading the SparkFun SMD soldering tutorials, and consider switching to a QFP prop, and SOIC eeprom. Soldering those should be a cake walk after that tiny NOT chip on your layout.

    Lawson
  • AleAle Posts: 2,363
    edited 2011-05-10 01:24
    Something that simplifies design of PCBs is to adhere to the rule "one side one direction for the traces". On top horizontals, on bottom verticals or the other way around. Decoupling capacitors are a MUST :)
    The Servo + seems to be connected to ground, at least to the EEPROM... have you checked that the schematic and the board are consistent ? (that they match ?)
    And a LED to indicate that power is applied to the board is a life-saver more than once :)... did you think about mounting holes ? they can be quite useful sometimes :)

    Edit: Have you built a prototype to check that everything works well ?... before committing to some PCB ?
  • LeonLeon Posts: 7,620
    edited 2011-05-10 02:00
    Posting the schematic would be useful, there might be other errors that aren't obvious from the PCB.
  • mhamen3mhamen3 Posts: 69
    edited 2011-05-10 09:33
    Thanks for the feedback guys, I really appreciate it.

    Schematic? Hmmm... I didn't make one. Did I mention this was my first time? Ha:innocent:

    I will be sure to add the decoupling capicitors to the prop, xbee, and drivers, and to finish routing the NOT and reset. Also, to change the ground connection for the eeprom: I would have totally missed that.
    And a LED to indicate that power is applied to the board is a life-saver more than once :smile:... did you think about mounting holes ? they can be quite useful sometimes :smile:

    I would like to add a power LED but I'm not quite sure how to do it. Simple I'm sure but its been a few years since I've taken electronics courses (I'm an ME) and anything outside of blackbox operation is beyond me. For mounting holes I have a lone one on the left and figured I could just use the holes from the regs on the right.

    As for the QFD prop, I thought about it but I already have a few of the DIP so I'm just going to stick with that.

    I'll revise tonight.

    Thanks again guys,
    Marc
  • Toby SeckshundToby Seckshund Posts: 2,027
    edited 2011-05-10 09:35
    I always like to put a earth plane on the top and bottom surfaces, if there are two, so that the ground impedance is reduced as much as possible an the extra screening can only help. It also gives the regulators something to use as a heatsink (it also means that there is less copper to etch away, and so the ferric chloride lasts longer).

    Although I have had no problems with it, it is generally recommended that there are no 90 degree track bends, use a short 45 degree bit. This is to prevent the etchant getting in and undercutting at the corner, I think.
  • LeonLeon Posts: 7,620
    edited 2011-05-10 09:37
    Always start with a schematic! It's the single most important part of a project's documentation, and makes it easy for someone else to check your design before you start on the PCB. PCB CAD software usually checks the PCB against the schematic, and informs you of any discrepancies.
  • JonnyMacJonnyMac Posts: 9,208
    edited 2011-05-10 11:18
    I didn't look very carefully but... 1) you seem to be missing pullups on the SCL and SDA line of the EEPROM, and 2) there are some right angles in traces that you may want to changed to 45s.

    And I agree with Leon: start with a schematic.
  • Nick McClickNick McClick Posts: 1,003
    edited 2011-05-10 11:23
    I would suggest adding a revision indication on the board ('Rev A' or whatever). A ground plane would be nice. And an unconnected plane under the Vreg's will help dissipate heat.

    Decoupling caps are a must: one for each Vdd - Vss pair. You can hide them under the Propeller DIP, if you plan on using a socket. Once, I assembled a panel of prop boards and tested each board before adding decoupling caps - just by testing, I ended up burning out the PLL's on about half of 'em.
  • LeonLeon Posts: 7,620
    edited 2011-05-10 11:36
    Just to see what would happen, I left them off a Microchip dsPIC board once and I couldn't even program the chip. It was OK when they were added, of course.
  • mhamen3mhamen3 Posts: 69
    edited 2011-05-11 07:33
    I didn't have a lot of time last night to revise the board. I do have some questions though.

    How difficult is it to make your own board (I have a small cnc mill). I have found a site ( www.pad2pad.com) that has quoted my board for just under $70 shipped for 3 boards. However, if I wanted to add the ground plane, BOOM, it shoots up to over $300.
  • JonnyMacJonnyMac Posts: 9,208
    edited 2011-05-11 07:34
    You might consider this guy -- I haven't used him yet, but my friends that have like his service:

    http://dorkbotpdx.org/wiki/pcb_order
  • LeonLeon Posts: 7,620
    edited 2011-05-11 07:50
    mhamen3 wrote: »
    I didn't have a lot of time last night to revise the board. I do have some questions though.

    How difficult is it to make your own board (I have a small cnc mill). I have found a site ( www.pad2pad.com) that has quoted my board for just under $70 shipped for 3 boards. However, if I wanted to add the ground plane, BOOM, it shoots up to over $300.

    Presumably that made it a four-layer board, which isn't necessary. It's very expensive, though, I can get them made much cheaper than that.

    Join the Homebrew-PCB Yahoo group if you want to make your own PCBs. I use photo-etch, it's very easy.
  • LawsonLawson Posts: 870
    edited 2011-05-11 08:43
    Yea, BatchPCB is where I go for prototypes if I'm not in a hurry. They're cheap for 1 or 2, have excellent quality, but take ~3 weeks to deliver. (and they'll happily cut out funny board outlines :D )

    All of my designs with ground plane have been two layer. For boards with a simple layout, like yours, you can often fit 95% of the non-ground traces on one layer. The second layer is then just ground plane, and short jumpers where two wires cross. I've got several boards designed like this that live near a Pockels cell. (switches 4Kv in a 1-2ns, unshielded it induces ~10Vp-p in a 3 inch loop of wire at ~4 feet.) Whatever noise that does couple into the power rails is unmeasurable. (<1mVrms with our oscilloscope)

    Lawson
  • Toby SeckshundToby Seckshund Posts: 2,027
    edited 2011-05-11 11:14
    When I surgested a ground plane I meant that one of the surface layers had the "gaps filled in" rather than a dedicated internal one. I use toner transfer and FreePCB so two layers are as complicated as they get. I wish I could get plated through holes though.
  • LeonLeon Posts: 7,620
    edited 2011-05-11 12:09
    There seems to be some confusion - what is being referred to as a ground plane is usually called copper pour. Ground and power planes are used on multi-layer boards.
  • mhamen3mhamen3 Posts: 69
    edited 2011-05-12 20:40
    Do I need 1K resistors between the xbee and the prop?
  • M. K. BorriM. K. Borri Posts: 279
    edited 2011-05-13 05:00
    Only if you want the prop to be able to turn the xbee on and off.
  • Toby SeckshundToby Seckshund Posts: 2,027
    edited 2011-05-13 07:52
    @ Leon Re:- Copper pour vs Ground plane

    That's true, I got it wrong. I wondered why there was such a leap up to more than the two easy layers. As I never get the chance to do commercial boards I had not considered internal layers.

    What I meant was copper pour, which can amount to 90% of the layer.
Sign In or Register to comment.