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.
For scale, the resistors are all 0603.
Electrical Engineering Stack Exchange is a question and answer site for electronics and electrical engineering professionals, students, and enthusiasts. It only takes a minute to sign up.Sign up to join this community
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.
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.
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.