Running tracks under SMD components (resistors and caps), is it good or bad?

[JPU]

Hi (thought Id start a new thread although kind of related to my last thread on space saving and programming SMD pics).

Im creating a PCB which I want to be as small as possible. I only have access to software which allows 2 layers only (freeware Diptrace). So I need to make use of the limited space I have. Instead of adding a mass of vias is it acceptable to run tracks under SMD resistors and caps. Im using case styles 0805 and the track widths are 0.3mm.

Thanks for looking.

 

[MartinM57]

OK physically or electronically?

Physically...http://www.digikey.co.uk/en/pdf/v/vishay/recommended-solder-pad-dimensions
...you have ~0.65mm between the pads of an 0805, track width 0.3, DIY-accessible professionally produced PCB (ITEAD studio etc) minimum clearance is about 0.2mm each side, so its very close/not feasible. Play around with the Diptrace Design Rule Checker...it's very good

Electronically - depends what signal is going through the 0805 and what signal is going on the trace under it. It could be fine, not recommended or just cause a big problem. You'd have to consider each one individually.

What's wrong with vias? I'm assuming your not DIY-making as running a 0.3mm trace through a 0805 outline is a big challenge.

 

[JPU]

The PCBs would be produced by PCBTRAIN (Newbury electronics). The resistor is used to clamp a picaxe pin to ground (10k) and the track is 5V logic signal. Nothing wrong with the vias I guess, I thought I might be able to make use of the natural bridge a SMD creates.

Diptrace design rule checker is flagging an error due to gap being too small when I have a 0.3mm track. However using a 0.2mm track eliminates the error.

 

[edmunds]

0.2 is perfectly ok. If you can actually keep the trace/space not less than 0.2 mm at any point, most board houses will give you the best pricing. Remember, that you can always increase the size of the cap/resistor if you need to get a trace through. I run a trace through 0402 components and two traces through 0603 and pay extra for my boards. 0.05mm trace is not impossible at all these days, but 0.1 is my standard signal trace. If you have to go less than that and if it helps, it is normally much better to go 4+ layers route and keep traces of normal width, just because a multi-layer board gives you a possibility for much better layout. And when you are paying extra for small traces, the extra money for multi-layer is not so important anymore anyway. It is very difficult to debug a board with 0.1mm trace if you need to get the solder mask off and stick a multimeter or worse - scope to the pin to understand what is going on. So, there are pros and cons as with everything.

It all depends on how much space really matters for your project. Your life will be A LOT easier if you stick to the standard rules of min 0.2mm trace and 0.3mm drill.

Edmunds