Take the 2-minute tour ×
Electrical Engineering Stack Exchange is a question and answer site for electronics and electrical engineering professionals, students, and enthusiasts. It's 100% free, no registration required.

I'm working on the second iteration of a board which uses quite a lot of 0402 caps for decoupling around processors. On the first version of the board I had complaints from the subcontractor that there was a lot of tombstoning on these caps, not in any particular pattern, just generally on the 0402 caps. They suggested that the 0402 pads seemed quite large. I'd used the standard 0402 reflow part in the Eagle RCL library which I'd assumed would be correct.

So, I've investigated further. I've looked at the IPC standard :

http://www.tortai-tech.com/upload/download/2011102023233369053.pdf

This land pattern is even bigger than what I was using and seems hard to believe. I've also looked at a selection of manufacturers recommendations on their datasheets for 0402 components :

http://www.yageo.com/exep/pages/download/literatures/UPY-C_GEN_15.pdf

http://www.vishay.com/docs/60119/landpatterns.pdf

http://media.digikey.com/pdf/Data%20Sheets/Panasonic%20Inductors%20Coils%20Filters%20PDFs/ELJ-RF.pdf

http://www.avx.com/docs/catalogs/cr05-32.pdf

There doesn't seem to be much consistency here other than they're all smaller than the IPC recommendation.

So, I'm confused. I really need to use 0402 caps as the tracking on this board is tight, but I don't want problems with tombstoning again. I'm particularly confused about this problem as I'd made a lot of effort with tracking on the 0402 caps to make sure the thermal paths to each pad were fairly equal so I'm pretty sure that's not the problem, I'm fairly convinced it's the land pattern that's causing the issue.

Has anyone got any recommendations, or even just an 0402 land pattern that's tried and tested working?

share|improve this question
1  
What does the actual board layout look like? –  Matt Young Feb 10 at 22:30
1  
My answer here to Should I worry about the risk of tombstoning? - with much of the useful material from elsewhere - is likely to be useful. A majorresource cited there is this 0402 & 0201 tombstoning report –  Russell McMahon Feb 12 at 7:20
    
Thanks Russell, that's a huge help. Probably the answer to this question to be honest. I've spent ages searching for information on this problem so I don't know how I've not come across that paper before. Interesting that it comes to the conclusion that pad sizes aren't a dominant factor in 0402 tombstoning. It also supports the suggestions of others in this thread who suggest that the subcontractor processes are the most critical aspect. –  Redeye Feb 12 at 19:36
add comment

3 Answers

Surface tension varies with the inverse of the bead radius, so I'd assume the smaller the pads, the worse the problem. Do traces enter and leave both sides of the pad exit with the same geometry? Were any of the 0402's on your board particularly prone to tombstoning? If so, that geometry might give you a hint.

Also, how experienced is the subcontractor? Is it a reliable and long-lived board assembly house with full size reflow ovens, or is it a "We'll print your board, and we'll populate it too" small business where you're not sure if they're populating by hand? Did they cut a stencil? Unequally applied paste can cause big differences in surface tension, resulting in tombstoning.

A place with a ton of experience and high throughput should be able to look at your Gerbers and find the trouble spots. Make them EARN those NREs! (Hey, "earn" is almost an anagram of "NRE"!)

share|improve this answer
    
Yes, the traces enter and leave the pad with the same geometry. No, there apparently weren't any that were particularly prone to tombstoning, it was just reported as a general problem. I think your comments about the subcontractor are probably fair - although I know the boards were made using proper stencils and screened by machine they don't do much work with such small components so maybe don't have the required experience for this sort of work. You're probably right - I need to get the subcontractor to earn their money. –  Redeye Feb 11 at 13:28
add comment

A bit of anecdotal information.. I had tombstoning problems on 0402 caps with the first run of a board.

Pointed out to the overseas assembly house, and had no further problems on many subsequent production runs (over 8 years now), with zero changes to the Gerbers. I made sure they understood that I was concerned about future runs, not assigning blame for a few fall-outs today, and they took care of us.

The size (Orcad SM/C_0402) was similar to the Panasonic datasheet recommendations:

a: 0.5~0.6 (Panasonic) 0.51 (SP 2005)

b: 1.5~1.7 (Panasonic) 1.63 (SP 2005)

c: 0.5~0.6 (Panasonic) 0.56 (SP 2005)

These days I mostly use the IPC wizard in Altium.

share|improve this answer
    
Glad to hear you survived using Orcad. I found it painful! –  Scott Seidman Feb 11 at 0:58
    
Every EDA program seems to be painful, just in different ways. I kind of miss the Orcad spreadsheet metaphor sometimes. –  Spehro Pefhany Feb 11 at 1:15
    
Yes, as with the comment above, I think you're probably right. I'll point it out to the subcontractor as a potential problem and let them figure out the best solution. –  Redeye Feb 11 at 13:30
add comment

Soldering 0402 caps shouldn't be a problem for your CM whether you follow the IPC recommendations or the manufacturer recommendations. Either you need a new assembler or your assembler should be able to give you very specific recommendations about what is causing the problem.

But just for the sake of fun, let's say that your assembler is your father in law and so you absolutely have to use his services.

I would say the first thing to check would be your thermals. If your thermals to a pour are too thick, then that pad might heat up more slowly than its counterpart. If you're seeing all of your caps tombstoning on the signal pad and not the GND side, that could be it.

Another thing to look out for is shadowing. If you've located those parts too close to the IC that they are bypassing, you might see that they tombstone on the pad that is farther from the shadowing IC. This can also happen if you don't space out discrete components enough. Some layout guidelines even recommend orienting discrete parts perpendicular to the direction of solder wave travel to avoid shadowing, but a decent manufacturer shouldn't have this problem.

Here's a screenshot showing the layout of a bypass cap and a resistor. To give you an idea of the dimensions, the distance between the centers of the two C16 pads is 42 mils. The pads themselves are 22 mil squares. The place bound is 55 mil x 96 mil. I've never seen a tombstoned resistor from our CM.

enter image description here

share|improve this answer
    
Thanks for the detailed answer - there's some really useful stuff for me to go and check on my board. For various other reasons I was going to use another assembler for the next run anyway. I think I need to use someone with a little more experience of this kind of board. –  Redeye Feb 11 at 13:36
add comment

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.