Cracked Via Barrels

[JivenJim]

I recently had three PCB's from two Board houses and three diffent designs having sporatic via's that have been failing after being stuffed and reflowed. The PCB's were 6 or 8 layer FR4 .062 or .093 inches thick. They were .012 inch thru via's with .024 annulars. And all PCB's were pre-E Tested by the board houses.

Now two of the three were with a new cheap board house, but the third was with a regular favorite. I can't think of anything that they're doing during stuffing to cause these Via's to fail only after reflow. And these seem to be very buildable Stackups. Is this a string of "bad luck" or do you know of anything that could be causing this? I did allow the isolated annulars removed and I've heard that keeping them in anchors the vias more. Of course this also increases chances of shorts with registree problems on internal layers. Any suggestions would be welcome.

Thanks,

Jim

[Cadcrusher]

What are you stuffing into the vias? And why would you do that?

[JivenJim]

Stuffing is a another term for Populating a PCB. (putting on the parts) No via craming here since college finals.

[Cadcrusher]

I know that usually parts aren't stuffed into vias.

[padmaster]

Is this the first time you've used this 24p-12d via padstack?

Are you tenting these vias?

Are they underneath a BGA?

What internal pad are you using in this via padstack?

Are you teardropping the internal pads?

[JivenJim]

No, we've use 24p-12d via padstack a few times before?

Not sure of term tenting vias. The Isolated inner Annulars were removed.

No BGA's but it's around a high count QFP's.

I've got the same 24P innternal with all inners teardropped?

[padmaster]

tenting = vias covered with soldermask


Here's the 24-12 padstack I use:

.018 round - top solder mask
.024 round - top
.024 square - internal
.024 round - bottom
.018 round - bottom solder mask


The .018 solder mask clearence allows for the barrel of the via to be finish plated. Maybe your not getting enough plating in the barrel of the via.

The internal square pads serve as a permanent teardrop, but if your teardropping, your probably not getting breakout.

[Ray from NJ]

Deleted

[JivenJim]

Hi Padmaster,

Interesting idea with the square internal pads. I verified that the solder masking is occuring after all plating thus, making the size to plating issue a non-factor. Typically I do not mask over the routing vias.

Ray, I'm using a 1oz copper on all layers with .5 oz plating and a 7/7 Trace space. (pretty normal right!)

Keep the ideas comming and Thanks!

[Ray from NJ]

Actually, 1/2 oz plating is where the problem could be.
Plating is not uniform in the vias. You get 1/2 oz on the ends of the barrel but could get down to 1/4 oz in the center.
Did you have a cross-section of the failed via done?

[robert Tarzwell]

your problem is the thickness of copper ver's the board thickness. As the board thickness increases the ability of the copper to stretch when the board expands due to soldering. A min plating for .o62 thick baord is 1.0 to 1.5 mils and I try for 2 mils in a ..090 to .125 multilayer. The shape and stack up of your pads has nothing to do with cracking of the via. Its a simple problem seen many times. as a note test I have done show improved resistance to via cracking with thicker palted copper. in fact over 3 oz there is no cracking no matter what you do to the board. Robert Tarzwell
megadawn.com

[padmaster]

Originally posted by JivenJim
I verified that the solder masking is occuring after all plating thus, making the size to plating issue a non-factor. Typically I do not mask over the routing vias.


If your doing SMOBC (solder mask over bare copper), the finish plating is deposited after the solder mask is applied. I recently went thru this with several vendors. They were screaming cause we were masking over smaller vias. They requested we open up the solder mask 6-8 mils larger than the finished hole size to allow for finish plating in the barrel of the via. Of course, as several members have stated, you should be plating external layers at least 1 oz. over nominal foil weight.

[JivenJim]

Did some more digging on the Plating. I found that they actually used .5 oz copper and plated 1 oz or .0013 inch (.033 mm), which should of put the 1 oz down the via. Sorry I told you the opposite before.

I asked a few PCB venders if they could plate thicker as Robert had mentioned. The feeling was that 1.5 oz plating was about as thick as you could get in to a .012 inch finished hole that the PCB house's drill at .015 inch and back plate to .012 inch. Robert: If you have any documents on this that could be posted explaining your results using 2-3 oz plating, it would be great to share with your online bud's. Sometime the boardhouse will preplate a few oz's of copper before they drill. Then Drill and add another 1-2 oz' before masking. This is done on high current stuff with finish weights of 4-12 oz's.

Padmaster: The "finish plating" is the normally HASL. (hot air over solder level) I was told this is very thin (around 3-5 micro-inches) so I don't think that would add any strength. Finishing information available on page 20 IPC-2221 table 4-3. As I understand it, the HASL coats the copper to protect it against oxidation before the board gets populated and reflowed.

These were great ideas's from both you guys that realy made my board house think. Still don't think I've found the smoking gun though.

[padmaster]

If your doing HASL, I hope these boards don't have a lot of surface mount on them.

And remember, the more you plate up the external layers, the more you have to increase your minimum spacing.

[robert Tarzwell]

in a nut shell the smoking gun is the plated copper thickness. If you do 5 solder float tests on the board then cross section I bet the vias are cracked. I found that the thicker the board the more the copper tends to crack. I also found that thicker copper can be stronger than the expansion forces of the FR4. I did have a similar problem on a .093 4 layer board, the assembly house did 2 or 3 solder cycles and the vias cracked, we plated a little more copper and end of problems.

For your board house, yes you can plate as much copper in the holes as you need, the trick is to start with 1/8 oz base copper ( or 1/4 for you scardy cats) then use a thicker dry film , which is available up to 4 mils thick, and drill the hole a extra tho or two larger and plate 2 to 2.5 oz of copper. then tin plate and remove the dry film just like normal. What they will find is very accurate lines, actualy fimer line can be produced using this method. With the extra copper i know the vias will not crack. We routinely plated as much as 12 oz of copper in the holes for power boards.
If you email me at rtarzwell@megadawn.com i can send you a copy of copper thickness verses solder cycles to cracking chart. I did try and attach the file test1.xls

[JivenJim]

Padmaster,
It's got about 1000 components on a 10X16 inch PCB, but nothing finer that 7/7. That seemed fine with the HASL although gold, or White tin would be nice. Good point on the min spacing being a factor of plating thickness/process. Maybe start a new threat if you got some goods on this.

Wow Robert!
Thanks for the Great info on your studies. This is the kinda great info sharing that makes the forum so productive.
I just got the word back from the QA department of the boardhouse. The cross sectional report showed that there were voids (cracks) in the barrel and adjoining sections were around .0008 inches thick or less, where it should of be .0016+ min. I like your ideas about using heavier plating. I would be concerned about overdrilling them to the point where drill accuracy would make breakouts the new problem. But everything is a trade-off for probable outcomes.

FYI the boardhouse said that an attributing factor was the useage of a conditioner bath known as Lea Ronal 1122 and / or debris remaining in the drilled hole. (as a pre-plating cleaning step. I think they called it D-Smear) They said that this cleaning chemical that was causing the inside of the drill holes to becoming slightly goo-ie. They are discontinuing the use of this coniditioner and using are now using a new blow/sucker machine to high pressure blow the hole clean prior to plating.

So as it goes, mulitple factors led to the Case of the Cracked Vias. As Designers armed with such facts, we will hopefully all keep our jobs a few more years ;+)

Thanks

Jim