13
\$\begingroup\$

I am (still) designing my first PCB and, according to prices listed on websites, the smaller the board the cheaper it is. That is, batchpcb charges per square inch. goldphoenix will print "as many as they can" on an 100 square inch board. Smaller is cheaper. Got it.

So should I try to cram as much as I can in a small space? Obviously one can go overboard doing this, but in all reasonableness, the point stands. Is there a standard guide for minimum distances between components? And are the standards based "this makes it easy to solder" or more technical problems (capacitances, inductances, sparks across components) that are too close together?

For example, one comment on this board from sparkfun says:

"These don't look like they're spaced at standard banana jack spacing. Isn't that important anymore?"

"its low current (5 amps) which shouldn't be enough to spark across the terminals at those voltages"

"I think the point is that most double banana plugs have a spacing of 0.75". The banana jack spacing on this board appears to be about 0.5"."

All implying that there the board has a poor design. But poor based on what?

\$\endgroup\$
  • 4
    \$\begingroup\$ That board might be a bad example, it's bad because double banana jacks have a standard spacing of 0.75", and this board doesn't follow that. It would be like designing a board with 0.08" headers; it's just not done without a good reason. \$\endgroup\$ – Kevin Vermeer Jan 22 '11 at 1:01
  • 8
    \$\begingroup\$ "its low current (5 amps) which shouldn't be enough to spark across the terminals at those voltages" This is shenanigans, current level doesn't even matter in this context, voltage will cause "sparking" not current. \$\endgroup\$ – Mark Jan 22 '11 at 2:17
6
\$\begingroup\$

Beyond constraints due to voltages or minimum trace/space widths (all important), on a larger scale the mechanical size should be convenient and conform to standards or convention if applicable.

For instance, regarding banana plugs, 0.75" is fairly standard for some adapters, so while 0.5" isn't inherently bad, it's possibly annoying to deal with.

Mounting holes should be easily accessible and fit common screw sizes (#4, #6, etc.).

Likewise, I strongly feel that a fairly popular prototype board is poorly designed because it has a non-integer multiple of 0.100" spacing between two of its headers.

\$\endgroup\$
8
\$\begingroup\$

There are IPC standards for component footprints. I recall that there are variations, roughly normal, larger and smaller. Those standards are based on "easy to solder with machine assembly".

\$\endgroup\$
  • 2
    \$\begingroup\$ landpatterns.ipc.org \$\endgroup\$ – starblue Jan 22 '11 at 11:21
  • 2
    \$\begingroup\$ IPC is an industry association of manufacturers that do work with printed circuit boards and electronic assembly in general. Their standards represent 'best practices' and are de facto requirements. You'll find that their procedures are almost universally followed by professional electronics manufacturers. \$\endgroup\$ – Adam Lawrence Mar 4 '11 at 18:59
  • 1
    \$\begingroup\$ The relevant standards are IPC-2221 (Generic Standard on Printed Board Design) and IPC-7251/IPC-7351 (Generic Requirements for TH/SMD Design and Land Pattern). \$\endgroup\$ – MV. Mar 25 at 4:16
6
\$\begingroup\$

For low-profile SMDs there's not really a limit. I've placed 0402 resistors as close as 0.1mm apart (spacing between pads). Higher components like connectors do require extra attention. You probably can't place a 0402 at 0.1mm from a 15mm high RJ45 connector, the pick-and-place machine may not be able to reach the position. Note that component orientation may matter! Talk to the assembly shop if you want to know what's possible.
Also worth noting is the clearance you have to keep to the board edge, again for the higher parts. If your panel is V-cut you need some space to fold the panel to break it after it's populated, preferably both up and down. RJ45s obviously go on the edge of a PCB, but don't place two of them directly opposite to each other on the panel if possible.

\$\endgroup\$
4
\$\begingroup\$

The vast majority of wires on a typical board are connected only to extra-low-voltage power and digital signals -- neighboring traces no more than 30 V apart.

For those components I have only 2 rules for the space between components:

  • space equal to height: I try to place components far enough apart so that I can inspect where the pins touch the board at a 45 degree angle. I.e., if I have a 0.5 inch tall component, the closest component is at least 0.5 inch away, so I can peek over the top of the tall component and inspect the side of that other component. (This also helps the fingers of robotic assembly equipment install some tiny SMT component, even if the robot was dumb enough to install tall components all around it first).

  • leave space for the PCB traces: with small SMT components, it's really easy to pack the parts together so closely that it's simply impossible to wire them all up with PCB traces, even at 0.006 inch (0.15 mm) minimum trace/space widths. When that happens, you're forced to push the components further apart to leave more room for traces between them.

I snap pin 1 of every though-hole part to a 0.1 inch grid -- i.e., pin 1 is some integer multiple of 0.1 inch away from the 0,0 reference point on this board. This makes it much easier to make a prototype -- and later, a test jig -- out of 0.1 inch grid prototyping board.

I snap the "reference point" (usually the centroid) of every surface-mount component to some grid -- perhaps starting out with a relatively coarse 0.05 inch grid (exactly 1.27 mm), but often switching to a finer grid. "PCB Design Tutorial" by David L. Jones and "PWB design flow layout" at the Massmind have a few tips.

Sometimes it's easier to leave twice as much room between components as your first estimate expects you'll need for the wires, just so you get something that's possible to route, and then afterward pack everything together once -- rather than needing to slightly nudge a quarter of the chips on the board a few dozen times while trying to push through a few hundred wires, getting some really long and winding routes when the "obvious" path is clogged.

Space equal to half the height exception: Since I can look "around" tall through-hole cylinder capacitors, I often leave a space only half their height around them (30 degree angle), hoping that the robot is smart enough to install them last.

Zero space exception: some connectors are designed to make a row of connectors each one practically touching the next -- a row of screw terminal connectors, a row of 3-pin hobby servomotor connectors, etc. So I lie to my CAD DRC and claim the whole row is one huge component.

If you have sensitive analog signals or high-voltage power or high-voltage signal traces, you'll want a little more space -- Wikibooks: Practical Electronics has a few tips.

\$\endgroup\$
2
\$\begingroup\$

In vague hand-wavy generic terms.

The voltage (or RFI / EMC) isolation requirements determines the spacing between traces and components. The biggest culprit of the second part may be inductors and transformers on double sided boards, for designers not use to doing analog design or layout. The component or module datasheet may have a keep-out area information as well as physical dimensions and restrictions.

Current (amperage) determines the PCB trace width, higher current means wider traces. This can often been single on a PCB with an on-board power supply and low-level digital components as an example in contrast. Large or oversize traces are occasional used as a heat sink in high-intensity LED designs by professionals, I do not believe it is commonly done by amateurs. I don't know if this is due to lack of access to thermal simulation tools or knowledge or some other factors.

The component layout and PCB manufacturing process are the ultimate guides for trace restrictions. For example the trace width and spacing on boards I intend for my own etching I give myself about double the spacing and width where possible to mitigate the risk of flaws in my process actually causing problems with the boards I make.

Some PCB manufacturers offer DRC (design rule check) file for supported CAD software that checks to ensure the board file complies with their technical manufacturing restrictions.

Various companies have tips and advice on PCB layout.

\$\endgroup\$
1
\$\begingroup\$

The minimum distance between components is obviously determined by how close you can place them, provided that you don't violate your board supplier's clearance between pads, and you are using typical voltages. You also need to provide room for the tracks between parts. You can use very narrow tracks and clearances between them, but that will push the price up, removing any savings you make on the board size. Like everything else connected with design, you need to come up with the best compromise.

The above applies mainly to things like logic. Analogue and RF designs are much more dependent on layout, and need special consideration.

\$\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.