Electronic – Should I worry about the risk of tombstoning


A colleague has (apparently unsuccessfully :-)) tried to convince me of the risk of tombstoning


in the following situation:

PCB detail

He claims pad 1 for R55 and R59 will lose heat faster during soldering because they have two traces leaving, while pad 2 only has one, and that this would cause tombstoning. Frankly, I've never noticed anything like it, even these 0402 resistors lay perfectly flat on the PCB. Am I too careless?

(The traces are 0.2mm wide)

I could also have shown 0402 parts with one pad connected via 4 spokes to a copper pour, which should be even worse, but again no problems whatsoever.

Best Answer


  • Tombstoning prospects increase with decreasing component size due to decreased energy of retention from surface tension forces compared to the self centering forces which will cause tombstoning if a mechanical imbalance occurs. 0402 appears to be about the point where you really start to care (although with due lack of care some manage it at 0603 :-)) and with 0201 it really matters. If you are "real enough" to be using 0201 you probably have other even more important matters to care about !

  • There are far more factors involved than just cooling rate, and it's very very much a case of "YMMV", but you'd be wise to pay some attention to your friend - while it's not necessarily liable to be an overwhelming issue, there are so many factors that if it happened to occur frequently in your case you would not be totally surprised.


Tombstoning, is contributed to by much more than just raw cooling rates - factors include pad sizes, pad shapes, solder used, solderability, surface roughness, paste type and brand, reflow profile ... and more.
Even Oxygen levels and use of an inert atmosphere can make some difference.

It's easy to pay slightly more attention to the issue when you get down to 0402 and below and thereby reduce the chances of having a bad day subsequently. It doesn't hurt to be aware of the issues even with 0603 components 'just in case'.

Here is a superb paper on the issue TOMBSTONING OF 0402 AND 0201 COMPONENTS: "A STUDY EXAMINING THE EFFECTS OF VARIOUS PROCESS AND DESIGN PARAMETERS ON ULTRA-SMALL PASSIVE DEVICES" which probably tells you more than you ever wanted to know. Results are based on a very large sample of tests (48 test combinations and 50,000 samples!). Interesting reading.

Here's a less useful but still interesting paper which concentrates on solder and paste composition and claims to solve the world's problems with appropriate formulationsPrevention of tombstone problems for small chip devices. Their idea of "small" is 0603 and 0402.

This paper Tombstone troubleshooting emphasises that there is no single cause or solution but also very clearly identifies differential cooling as a significant issue, with an example image that is uncomfortably close to your one for practical purposes:

enter image description here

              Pad 2            Pad 1 
  • They say: if Pad 1 is connected to a wide trace, ground plane, or other heat sinking element. Pad 2 is connected to a thinner trace or less massive circuitry element. Pad 2 will often be hotter than Pad 1 and reflow before Pad 1. This temperature difference result in a reflow timing difference. When Pad 2 wets first, the wetting force from Pad 2 may be enough to overcome the force from Pad 1 resulting in a tombstoned component

This July 2011 white paper agrees with your friend. The Low Mass Solution to 0402 Tombstoning

In summary it says:

  • Variations in the components [thermal characteristics] must be accounted for in the pad geometry, or else tombstoning may occur. He also recommends treating each pad as a group, and ensuring the copper density of each pad is equal (or very close), meaning both pads achieve the same temperature and liquidus at the same time. Also, Reno says, both pads should achieve solder flow to exposed copper at the same time, and be equal in solder volume necessary to control capillary action.

enter image description here

More of the same

SMT net discussion - more of the same. Horrendous :-)



  • MD = metal defined. Relates to PCB pad. Whole of available metal area is pad with no solder mask limiting pad extent.

  • SMD = solder mask defined. Metal extends beyond pad area defined by solder mask.

  • YMMV = your mileage may vary = caveat emptor = what you experience may be different to what I experience etc. USA origin. It's a wry comment, almost a cynical joke based on US auto advertising claims. viz In our test Model XXX auto got 56 mpg on an urban cycle driving test - YMMV. ie While WE got 56 mpg, you may not.