7
\$\begingroup\$

Are these traces too close for conventional PCB manufacture? DRC check advises against it, but I haven't filled out all the settings for it.

alt text

For scale, the resistors are all 0603.

| improve this question | | | | |
\$\endgroup\$
  • 6
    \$\begingroup\$ Setup your DRC rules with what ever fab method you are going to be using requires. Then work on removing all DRCs. \$\endgroup\$ – Kellenjb Oct 24 '10 at 18:10
  • 2
    \$\begingroup\$ Why do you want them so close and so small? You can make your traces just about as small and close as you like, but you're going to pay for it. I use 12 mil if I don't have a compelling reason to do otherwise. \$\endgroup\$ – Kevin Vermeer Oct 24 '10 at 21:39
  • 1
    \$\begingroup\$ Because I'm working on a small 40mmx60mm board, every mm is precious. \$\endgroup\$ – Thomas O Oct 24 '10 at 21:41
19
\$\begingroup\$

It really depends entirely on what the signals are carrying and what the manufacturer says they are capable of.

The general rule of thumb is that you should maintain a minimum of the width of the trace. If you are using 10mil traces, then you should also have 10 mil of space between them. If your traces are carrying sharp-edged waveforms (i.e. square waves, digital signals, data buses) or sensitive networks (A/D, sensor or op-amp inputs) then you want to maintain more of a distance and perhaps add a guard ring (ground traces) on either side of the trace in question.

I am a (very) happy customer of Sunstone; their manufacturing process allows me to use 5 mil trace with 5 mil space without any trouble, and they can do 3/3 if you're willing to pay extra. A 5 mil trace is a damned thin trace and pretty much at the level of most commercial boards these days, so there is little reason to go thinner unless you have some specialized application. For most of my boards I try to stick to 8, 12 or even 16 mil traces since they're much more rugged and easier to work with should you have to modify the board. If you're carrying high current or routing supplies I will make the traces as wide as I can afford to, from a board real-estate perspective. Wide traces are good.

I see from your picture that you're running traces between the pads of 0603 components. This isn't verboten, but it's also generally something you will want to avoid. It's too easy to end up either bridging some solder to the trace underneath (soldermask failure) or damaging the trace if you have to lift the component off (e.g. a bit of flux sticking under the part and effectively "gluing" the trace to the bottom of the component. The trace from R15 also goes awfully close to the pad for R8, and the trace that goes around the top right-hand side of the board seems to come awfully close to the via. It would be wise of you to find out what the board manufacturer is capable of doing, and what the recommend (these are not the same thing) and programming that into your layout's DRC. If the DRC flags something, fix it. This is Design For Manufacture (DFM) 101. If you violate the DRC you end up with higher manufacture wastage and in the end, more expensive boards. Sunstone is really nice here; they provide eagle-format DRC rule files. You simply download it and use them.

The DRC can be a real pain in the ass, but it's like eating your veggies; your project will be better off for it in the end.

| improve this answer | | | | |
\$\endgroup\$
  • 1
    \$\begingroup\$ Great. Thanks for your answer. Good point on the wire next to R8 and the via, I am able to spare the space for them so I will actually move the. \$\endgroup\$ – Thomas O Oct 24 '10 at 17:49
  • \$\begingroup\$ Are the traces too close for 50V signals maximum? \$\endgroup\$ – Thomas O Oct 24 '10 at 17:50
  • 1
    \$\begingroup\$ Andrew was focusing on the effects of putting a high speed signal in close proximity to another trace. Coupling will occur results in crosstalk. Voltage is a different can of worms. With voltage you will need to be concerned about arching between 2 traces. This will change depending on the fab process. smps.us/pcbtracespacing.html talks about the spacing required. \$\endgroup\$ – Kellenjb Oct 24 '10 at 18:23
  • 1
    \$\begingroup\$ it's unlikely he is going to encounter anything that will have to worry him about creep and strike distances, but you're right, if he has to worry about ringup voltage and such he's going to have to take those into account when designing the distance between traces. \$\endgroup\$ – akohlsmith Oct 25 '10 at 0:53
5
\$\begingroup\$

You are setting up DRC at the wrong end of the process.

Whether you set the DRC values to reasonable values (for an open-source project) or specific values for a particular manufacturer, you need to do it at the beginning of a project. Then you run the DRC checker periodically during layout and keep it DRC-clean.

Most pcb layout software, including the one you are using, includes an option to "auto-enforce DRC clearance." This option will help you keep out of trouble.

Now you are at the end of the layout trying to fix up DRC at the end. This is going to be a pain. You may end up re-laying-out most of the board.

Experience is a hard teacher, the lessons come after the tests.

| improve this answer | | | | |
\$\endgroup\$
3
\$\begingroup\$

Andrew's answer is spot on for general routing.

There are some other aspects that are worth knowing even if they are not relevant for this application, is clearance for higher voltages and low pressure (high altitude). EN60065 is a good starting place for higher voltages and mains voltages as it gives minimum clearances required for commercial equipment. In one of my previous roles, we did designs for avionics systems and the clearance required become much larger due to the reduced air pressure, hence reduced insulation between traces.

One method of increasing insulation is to use conformal coating. This has the added advantage that the insulation will not change over time, compared to an uncoated board that has dust and dirt settle on it. Dust and dirt will reduce the resistance, and may lead to short circuits between higher voltages traces. Hence the requirements of EN60065.

| improve this answer | | | | |
\$\endgroup\$
1
\$\begingroup\$

My own personal rule-of-thumb is 3x trace width between generic traces and 5x trace width for "noisy" traces (clocks, etc)

| improve this answer | | | | |
\$\endgroup\$
  • \$\begingroup\$ 3x trace width seems overkill to me. I use 1x on traces 0.2 mm wide or wider. \$\endgroup\$ – stevenvh Aug 14 '12 at 10:51
1
\$\begingroup\$

You should avoid acute angles where tracks meet pads; I can see one near the centre of the image, and you might have some more on the rest of the board. They can cause problems in manufacture, and look ugly.

| 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.