6

After filling a bunch of breadboards with some successful experiments, I'm ready to start making PCBs and I'm wondering if there are any design considerations of which I need to be aware?

Some PCBs I've seen are spacious with long traces. On others, components are packed like sardines. Before I go packing a bunch of stuff into the minimum space possible on a PCB, are there any considerations apart from the ones listed below of which I need to be aware?

DETAIL: Since I'm using toner & cupric acid to etch the boards, I know I can't have crazy thin traces or spaces between them.

HEAT: I need to leave ample space for air circulation so I don't fry my circuit with heat buildup. However, I see this more a factor of enclosure (e.g., big enough to allow circulation or a fan if deemed necessary) and heatsink choices.

What else should I know?

JYelton
  • 32,302
  • 33
  • 134
  • 249
dwwilson66
  • 3,402
  • 11
  • 33
  • 42
  • 2
    Digital? Analogue? High speed? High voltage/current? Special low noise requirements? – pjc50 Dec 17 '12 at 12:58
  • 1
    That's the kind of question that can be answered in a book. – Vladimir Cravero Dec 17 '12 at 13:03
  • @VladimirCravero - that's what I was afraid of. :) – dwwilson66 Dec 17 '12 at 13:18
  • @pjc50 - all good questions....For the PCBs I'm doing now, they're all analogue, none will exceed 36VDC/2A, and while they are audio circuits for synthesizer input (VCOs & Noise Generators) and noiseless is preferred, a noisy circuit may yield interesting effects. I did not design for any speed, so I'm guessing it's not high speed. – dwwilson66 Dec 17 '12 at 13:27
  • @VladimirCravero - Do you have a good book recommendation for a newbie? – dwwilson66 Dec 17 '12 at 13:28
  • I don't think such a book exists... I mean, it's all about experience. I'll try to give some suggestions as fceconel has done, but I'm not able to cover the whole topic. Your clarifications are useful though. – Vladimir Cravero Dec 17 '12 at 13:35

3 Answers3

8

I'm going to say "Location, location, location". You can make or break a PCB by selecting where the components go. Some (like switches, or transistors that have to be on a heatsink) may have fixed positions; but you can make a huge difference by moving the rest around until they are in the best place. Actually routing the signals is less difficult!

Some components call for placement close together to minimise the length of high current paths. That can also make the difference between a nice quiet board and one that fails EMC emissions tests.

Some components call for the right orientation to connect to their neighbours without all the tracks crossing over each other. Or enough distance between them to allow all the tracks to pass. And so on.

Spend time placing the components, watching the "rats nest" pattern of unrouted traces, and simplifying it as much as you can. Make several trial placements and save them, and route the best. When you get stuck, move the problem parts around and start routing again.

It really does take practice.

Minor points :

  • if the boards are to be hand assembled, there will be many fewer mistakes if all the ICs and polarised caps are the same way round!
  • if all the components are on the same side of the board, build is easier
  • you can simplify testing if every signal has at least one accessible pad (test pad or existing IC pin or socket pin) on the opposite side of the board...
6

If you're designing low-freq boards (e.g. some MHz or below) I don't think there's much more to consider. I'm assuming it's not high-voltage also, obviously.

Keep the space between traces wide enough that you won't accidentally short when soldering (or if it happens, that it's easy to remove the excess). For the traces themselves, there are many trace width calculators on the Internet, like this one.

For simple transistor & TH IC boards, I generally use 0.5mm trace-and-space (20 mil). These are almost always enough unless you need high power (in which case you can calculate specifically) and easy to produce good results with thermal transfer - my preferred method for single-side, basic boards.

Given that, the other things I consider are:

  • The placement of external connectors, heat sinks, etc. related to the case
  • The relative placement of the components to minimize trace lengths
  • How easy it'll be to solder and remove any of them
  • How much spare space there is for the traces - and jumpers, if needed
  • How long are the traces on average, and are there higher speed traces unnecessarily long

I generally start with a bigger board than needed, use the autorouter to get a sense of where traces can go and how much of the board is filled up, then remove the traces, adjust the relative position of components, reduce the board to what I believe is the minimum, and autoroute again. When I arrive to the minimum board that's still comfortable to work with, I route manually the traces.

fceconel
  • 2,659
  • 22
  • 19
4

This is a response to the O.P.'s comment/request for books:

  1. IPC standard IPC-2221 Generic Standard for Printed Circuit Board Design.
    1998
    Must read. The 1998 version of the standard can be found on the wed free of charge. The 1998 version is adequate for introductory purposes.

  2. Kraig Mitzner. Complete PCB Design Using OrCad Capture and Layout.
    2007
    ISBN-13: 978-0750682145
    Even through the title emphasizes use of OrCAD tools, the first portion of the book is a general overview of PCB technology.

  3. IPC standard IPC-2152 Standard for Determining Current-Carrying Capacity in Printed Board Design.

  4. Donna Dearinger. PCB Fabrication for Designers.
    2003
    Printed Circuit Design, pp.10-11, UP Media Group Inc

  5. Dan Beaulieu. Printer Circuit Board Basics.
    ISBN: 0-9743561-0-7 (4th ed. 2003)
    Basic processes used for PCB fabrication in the industry.

Nick Alexeev
  • 37,739
  • 17
  • 97
  • 230