3
\$\begingroup\$

I'm an EE graduate who enjoyed the first taste of designing and fabricating hardware. My first board was a really low speed microcontroller board using mostly DIP and through-hole components, like something straight out of the 80s. It's very easy to translate to a PCB from a breadboard using these packages, but they are large and cost per square inch is very high for single-digit run project boards. To cut down on costs I designed a board using solely SMT components which was far more compact (as well as complex) than any other previous board I've made. I'd like to verify as much as possible that my designs work before spinning a board so I don't waste my limited budget (and have to delay for the new boards).

What verification practices should I use, besides making a breadboard facsimile, when making a (low speed) PCB? Up until now I've just made sure everything was routed, passed DRC and ERC and hoped the board works. I feel like there's more I should do.

\$\endgroup\$
  • 1
    \$\begingroup\$ Test points test points test points test points test points ... and remember to have a good point to tie o-scope ground clips to. Not that this means the board will work, but if you have important things broken out, you also have nice points to solder wirewrap wire to when you get to the cut-trace-and-jumper stage! \$\endgroup\$ – Scott Seidman Jan 11 '14 at 0:22
5
\$\begingroup\$

My answer is more for obsessively checking your first (or second) personal "low speed" PCB rather than verifying your design.

  • Make sure your DRC is checking for off page connectors
  • Print out the datasheet pages for each IC/transistor etc and go through with a highlighter and verify every pin against the pin on your schematic.
  • Do the same obsessive check with your layout
  • Check all three pin devices like transistors against their diagram in the datasheet make sure that the pin numbers on your PCB are correct. It's easy to do these SOT-23 style devices wrong ( I usually draw a diagram for my layout guys).
  • Do a similar check for polarized components, did you get diodes correct and are they marked which way they go in? What about polarized caps?
  • Is this a four layer board? No? It probably should be :) signal-gnd-power-signal Even at low speeds this will help you. Sometimes you just gotta go 2, but do it because you know the consequences or that it won't hurt you.
  • Open your gerbers/drill in a gerber viewer like the free GC-Prevue, now print them to a laser printer 1:1. Order your more complex parts and see if they fit on paper. Is it perfect? No. Will you catch using the wrong footprint or wrong spacing? There's a good chance of that.
  • What did you do for power did you verify your regulators can supply enough current? How about how much heat they will burn off trying to do it? How about power dissipation for a linear regulator or switchers fets. You want to make sure you don't burn them up. We could go deep into the power section but I'll leave it at that.
  • Sounds like your design is cost conscious, consider only mounting parts on the top of the PCB. It will save a whole step during automated assembly if that's where you hope to get to, and that will lower the price.
  • Make sure your gerbers files are clearly labeled for the fab house, a drawing usually helps showing what layer goes where, some people go as far as labeling the layers in copper to make sure it's done right.
  • If possible have someone else review your schematic and pcb, peer review, peer review.
  • Have your 30 Gauge rework wire handy for when the boards come back, I like to use blue for rework :)

The list goes on but I'm tired and I hear the baby crying :) Hope some of that helps.

| improve this answer | |
\$\endgroup\$
  • \$\begingroup\$ Excellent advice. Printing 1:1 definitely saved me some part alignment issues on my last board. I just want to add that you should always check that the flanges of TO-220 parts are insulated if they share a heatsink, since quite often they're electrically connected! \$\endgroup\$ – BB ON Jan 11 '14 at 15:18
5
\$\begingroup\$

If the unspecified circuit is analogue or digital logic then using a simulator is a definite thing to do. There are quite a few free simulators around and LTSpice springs to mind. It's a relatively steep learning curve but totally worth the effort.

If it's a micro based design then I can't offer help other than to suggest you double check every pin. If it's an EPLD, then double check the pins and run simulations of the logic within the suite of tools usually provided by the vendors.

| improve this answer | |
\$\endgroup\$
  • \$\begingroup\$ Ah, yes, I didn't specify; I implied digital circuits. \$\endgroup\$ – BB ON Jan 11 '14 at 0:11
  • \$\begingroup\$ My answer still stands I believe. \$\endgroup\$ – Andy aka Jan 11 '14 at 0:14
2
\$\begingroup\$

You can't totally your PCB/Board before you have it in your hands. But here are some tips:

  • Simulate important functions or double check the computation if you can't simulate easily.

You should know what to expect of a function from your design/computation, the simulation will give you a result, it may fail. In this case, double check your computation, if it is ok, then you made a mistake in your simulation.

(That's what Andy aka recommand)

  • If you have expensive and/or hard to solder chips (CPU, MCU), put some buffers on I/Os that have an exterior connection (typically JTAG, programmings I/Os). If you have a misconnection or overvoltage, the buffer will break and not you expensive chip.

  • We always miss something, so be prepared:

    1. Make important signals accessible with a test point or a via
    2. Plan wire connection, if you have some BGA/LGA, by having some holes to pass the wires
    3. Plan spare footprints: if you have pull-up on some signal (resets, I2C, SPI, etc), plan a "pop/no-pop" (personnal term) : make a pull-up and pull-down footprint, but you will only solder one resistor. But if you have some troubles, you can easily check if the invert works better. This small tricks saved me some times :) It can also be applied when you have some resistors/capacitance with specific values (sensing, mosfet snubber, etc.) plan 2 footprints in series for resistors and two footprints in parallel for capacitors : you will be able to adjust more precisely the value by combining two components. http://www.toopix.eu/userfiles/370a6ae646fef1ab7817062da94f58d3.png (Here the pop/nopop is used on a hardware configuration 4-bits word, but it's just to show you on a schematic)

    4. If you have multiple power supplies on you can use 0 (zero) Ohms resistors to isolate them at the bring-up: you will solder the resistors step by step, verifying that each supplies is compliant. We used this on a complex board with FPGA, CPU, DDR, QDR, PHYs, etc. we had a complex power supply function and to avoid destroying a chips we powered up each power supply one by one.

  • Finally: peer review

You are not perfect, so try to gather some feedback from fellow students or professors. Maybe you missed something huge, but 2 or 3 people, generally can't miss huge mistakes.

| improve this answer | |
\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.