Electrical Engineering Stack Exchange is a question and answer site for electronics and electrical engineering professionals, students, and enthusiasts. Join them; it only takes a minute:

Sign up
Here's how it works:
  1. Anybody can ask a question
  2. Anybody can answer
  3. The best answers are voted up and rise to the top

In order to reduce the size of a PCB I will probably have to use smaller SM components. I currently use mostly 0805 passives, and am thinking about going to 0402 or smaller. Apart from power dissipation considerations, any pitfalls I should be aware of when making the transition?

The assembled boards will be made by a specialist contractor

share|improve this question
1  
how good your eyesight is :-) – Icy Jan 29 at 11:15
2  
Don't sneeze! Beware of the voltage limitation of resistors, and also look out for capacitor voltage coefficients. When capacitors are made very compact, even X7R may have very large value drops at full working voltage. – user1582568 Jan 29 at 11:43
3  
I think tombstoning can be more of an issue because of unbalanced surface tension, but that's just a feeling based on a handful of instances – Scott Seidman Jan 29 at 11:44
4  
just a note: you can't put a trace between pads on 0402 while you can on 0805, this may make routing more difficult. – Cano64 Jan 29 at 14:45
1  
@Cano64 most of the time :). If you're working with 5mil trace/space, you ought to be able to squeeze a trace through if things are really cramped. – uint128_t Jan 29 at 16:14
up vote 7 down vote accepted

0402 obviously is harder to hand assemble. I am young (<30), moderately near sighted (-4.5) and have a reasonable steady hand. I can hand assemble 0402 boards without magnification, but it is very tiresome to do them for hours on end.

If you need to get them assembled by machine; make sure that:

1) Your assembler's pick&place machine can even handle 0402 at a good rate & yield. Some assemblers may charge more because they are forced to run the boards through one of their more modern machines.

2) Double-sided load. Some boards just need this assembly step, like BGA often puts decoupling caps on the bottom of the board. However some assemblers have trouble with 0402 components on the bottom side of the board. They may force you to keep it at 0603 or greater. The risk is that 0402 components will slip of the board in a 2nd reflow cycle.

3) Electrical properties. Obvious one is of course power rating of resistors. Voltage rating is also likely worse, because of the physical smaller dimensions. But also consider the voltage bias degradation effect of ceramic class 2 capacitors; for smaller packages in same voltage/capacitance this effect may be worse.

On the other hand, some properties like lead inductance is lower. In addition sometimes you can put capacitors right at the chip pins for QFP style packages, while routing signals underneath the chip. In effect the loop area for the decoupling capacitor is much much smaller than a larger size capacitor that may be placed further away to comply with signal routing.

share|improve this answer

Your Answer

 
discard

By posting your answer, you agree to the privacy policy and terms of service.

Not the answer you're looking for? Browse other questions tagged or ask your own question.