EDA > General PCB/EDA/CAD Discussions

Stop using 0603 or bigger resistors and capacitors?

(1/4) > >>

Due to the shortage of 0603 and bigger resistors and capacitors, its recomended to use 0402 and lower. (where power levels/voltages allow)
This seems a bit drastic doesnt it?
Is the manufacture of 0603 and bigger resistors and capacitors so complex that extra plants wont be set up to produce them?

0402's are terrible as resistors have no value on them, and they seem to tombstone/head-on-pillow  more.
(unless you have massive PCB runs where you can tweak the solder bath temperature and ramp profile to eventually get it perfect every time)

I don't have any insight about the supply problems.

Yeah finding ones with markings is not always easy, though I seem to recall seeing some 0402s that are marked from some vendor(s).  Perhaps a bad memory.

As for tombstoning, though, there's no good reason that should happen with good PCB design and soldering technique:

1: Design pads per. IPC or vendor suggestions for size and shape and spacing.

2: Design solder paste mask per. vendor suggestions for layer thickness, aperture size/shape/vs. land pad size and type of solder.

3: Make the thermal environment and effective wettable pad area the same for both pads.  E.g. if a pad is connected to a plane, use thermal relief so the other pad's connections and heat sinking will be similar in width and conductivity. 

4: Make trace / net to pad connections symmetric -- If one trace exits the pad with say 0.2mm width, make the other pad's trace / net connection do the same from the corresponding edge of the pad.  Don't make one pad exit sideways and the other pad exit from the end or the opposite side.  Symmetry.

5: Preheat your boards and follow the ramp-up to reflow profile approximately so the pads will have generally equal temperatures as the soldering begins before reflow and equal cooling after reflow.

6: Use smaller traces (neck down) when they enter the pad so the size of the trace is significantly smaller than the pad at least within the area where the solder mask is open around the pad.  i.e. keep it symmetric and don't let one pad's solder wick off to a large trace / plane much more so that will happen on the other pad.

You should have no real problems with 0402 in these ways even for manual rework without using a paste stencil.

Yeah, "vendor suggestions" is the right thing to do. For professional and/or high volume production your assembler is most likely able to tell you what footprint geometries work best, i. e. reduce the probability for tomb-stoning. And that is not necessarily an IPC compliant footprint.

I've been using 0402 parts for years now pretty much everywhere (except where larger parts are required due to voltage/current/power regime). Didn't notice any excessive tombstoning compared to larger parts. But they are much more convenient for layout due to their small size, as space on multi-layer boards is always at premium.

0402 and smaller are hard to handle (well, 0402 is still OKish) for hand soldering, but otherwise, they are fine.

Of course, 0402 can be used only if you don't exceed its max power rating, which is significantly lower than for 0603 for resistors. So it's not possible to replace those in all cases.

As far as tombstoning goes, I've never seen any issue with 0402. You'd probably have to deal with a pretty bad PCB design for this to happen. OTOH, 0201 is a lot trickier.


[0] Message Index

[#] Next page

There was an error while thanking
Go to full version