Repair of BGA - solder balls melted down via holes

Go To Last Post

31 posts / 0 new

Author

Message

nkinar

Level: Hangaround

Joined: Wed. Jul 18, 2007

Posts: 399 View posts

Location: Canada

Posted by nkinar: Tue. Mar 22, 2011 - 03:33 AM

I've created a new prototype circuit board with 217-LFBGA (AT91SAM processor) and 54-VFBGA parts (SDRAM memory). Unfortunately, I've found that some of the through-hole vias were too close to the BGA pads, and during reflow, the solder balls melted down the via holes :(

This is clearly shown on x-ray images of the PCB.

For the next revision of this prototype, I need to move the vias further away from the holes. Alternately, I've been told that I could "tent" the vias so that the holes are filled, but this may raise the cost of the PCB.

The problem is not too bad; approximately 10 pads per BGA are affected, and most are electrically connected :D

The real showstopper is that one of the pads is completely unconnected. This pad corresponds to "D5" on my SDRAM memory bus. I've written test programs, and these programs show that there is indeed an issue with reading and writing to this data bit. Moreover, this pad shows up as completely unconnected on the x-ray images.

I'm working on the PCB for a research project, and I would prefer to salvage this PCB so at least I could create a working prototype.

Any suggestions? I would be extremely interested in hearing about recommendations as to whether there is a board rework/repair facility somewhere in Canada (or even elsewhere in the world) that could successfully repair this PCB. Is there anything that I could do myself? I would prefer getting this taken care of as quickly and efficiently as possible.

As an aside: Although the main microcontroller being used in this system is an ARM9, there are two other 8-bit AVR parts on this circuit board, so I haven't abandoned the AVR architecture at all :wink:

Tags:

Learning and Information, General Electronics

dksmall

Level: Raving Lunatic

Joined: Mon. Apr 16, 2001

Posts: 3676 View posts

Location: Phoenix, Arizona

Posted by dksmall: Tue. Mar 22, 2011 - 04:50 AM

How is the D5 pad not connected? No solder ball contact? Or was the board not routed properly? Was any kind of DRC run on the layout?

nkinar

Level: Hangaround

Joined: Wed. Jul 18, 2007

Posts: 399 View posts

Location: Canada

Posted by nkinar: Tue. Mar 22, 2011 - 05:02 AM

dksmall: The D5 pad is not connected due to a lack of solder ball contact; most of the solder ball melted down the via hole. As far as I can tell, the board was routed correctly, and I did run a DRC on the layout.

glitch

Level: Raving Lunatic

Joined: Sat. Jan 12, 2002

Posts: 8696 View posts

Location: Canada

Posted by glitch: Tue. Mar 22, 2011 - 05:12 AM

where in Canada? I'm in Toronto and may be able to help you out. One option is to reflow the chip again, or to replace it altogether. Depending on the via diameter the pad could be reflowed from the backside, and a wire pushed up to try and push/bubble the solder back up to the pad.

Tenting via's should not increase the cost of the PCB, as all you are doing is omitting holes in the LPI [solder mask] where the via's exist. Some vendors may do an inspection/repair pass to touch up the LPI over the via's in any locations where it opens up, if they do this, there may be a minimal charge to do so. [alternatively they blindly apply a 2nd layer to the via locations]We do it as standard practice for our production boards, so that should give an idea of how minimal the cost impact of tenting is. [in fact I don't think we are seeing any up-charge from the vendors we use]

As this is a research project [ie one off] any added cost of tenting should not be an issue.

Writing code is like having sex.... make one little mistake, and you're supporting it for life.

nkinar

Level: Hangaround

Joined: Wed. Jul 18, 2007

Posts: 399 View posts

Location: Canada

Posted by nkinar: Tue. Mar 22, 2011 - 05:32 AM

Thank you very much for your response, glitch!

glitch: I'm here in Saskatchewan, just a few provinces over. Anything that you could suggest would be greatly appreciated - I am not very familiar with BGA manufacturing processes, and I am not immediately certain what would be the best way to proceed.

The via diameters are no less than 8 mil drill, and the PCB has at least 5 mil trace width/spacing. I've never heard of reflowing the pad from the backside, but it sounds like a very interesting idea. How could I do this, and where would I find small enough wire? Is it best to do this myself with hot air and a pre-heater?

Perhaps I could flip the circuit board over so that the BGA part faces a Hakko FR-830 hot air pre-heater element. Could gravity pull the solder down? Or would it be beneficial to still use a wire? Perhaps some No Clean flux could be applied before pushing a wire through the via?

According to my PCB editing software (Altium Designer) I've omitted holes in the solder mask, but unfortunately the vias are still "open." Is "tenting" different than plugged vias? Looking at the circuit board, there are still holes that I can see through.

meslomp

Level: Raving Lunatic

Joined: Wed. May 2, 2007

Posts: 5714 View posts

Location: Nieuwegein, Netherlands

Posted by meslomp: Tue. Mar 22, 2011 - 06:36 AM

tenting vias means that you put solder mask over them. If you look at your output data the soldermask layer should show no via holes.
If you have tented the vias then it should not be possible for a via hole to be flooded with solder. So it might be that your board manufacturer has editted your gerbers......
Or the via holes are inside the pad (which should never be done with a BGA, you know why not now))

If you flip the board and heat it till the solder melts, what will happen you think??? keep in mind that the components are smart enough to understand what to do when gravity starts pulling at them.

we have wire like:
http://nl.farnell.com/pro-power/rrp-c-105/wire-copper-1-0-15mm-pk4/dp/146182
that should fit.

you could selectively heat the via that is giving you problems by using a hot air gun. It is not ideal for production and the PCB, but could make back the contact. specially if you put a piece of the above wire in the hole.

glitch

Level: Raving Lunatic

Joined: Sat. Jan 12, 2002

Posts: 8696 View posts

Location: Canada

Posted by glitch: Tue. Mar 22, 2011 - 06:48 AM

yes tenting and plugging are two different things. With tenting you may still see through the holes, but due to the LPI being around the hole, and partially in the hole walls, it should not draw in solder from a near by pad, unless there a fair amount of overflow during the reflow process. Plugging, on the other hand, involves a pass where the via holes are literally filled with solder.

As for heating from the back side, That is based on a via [that falls very close to the pad, and is part of that net] being present. Pre-heating the board is a necessity. Wire wrap should be able to push through an 8 mil via, but barring that, you use a single strand from a finely stranded wire.

Having said that, I would first reflow the chip, as it sounds like you have access to a re-work station. Pre-heat the board, and then heat the BGA until it starts to float. Give it a few light lateral pokes with some tweezers on the edges so that it is centred via surface tension of the molten solder. Then give it a light push or two directly downward so that any non-contacting points make contact with the pad below... they will remain connected as the BGA rises back up forming a solder column, and that's it. If you have a very thin [no clean] flux, you can try applying it under the bga by flooding the area around the chip. [apply int on one side, and then tilt the board so gravity draws it under the chip until it begins to run out on the opposite side. Repeat the process with the other edges, though you won't be able to visually tell, so just go by gut based on the time on the first pass] This will help with the reflow process. If the flux is too thick, don't waste your time.
If you are concerned about the vias under the BGA, you can plug them manually your self with a soldering iron, do this before re-flowing the BGA.

Writing code is like having sex.... make one little mistake, and you're supporting it for life.

nkinar

Level: Hangaround

Joined: Wed. Jul 18, 2007

Posts: 399 View posts

Location: Canada

Posted by nkinar: Tue. Mar 22, 2011 - 03:17 PM

meslomp: Yes, looking at the data it is clearly shown that there are no via holes on the soldermask layer, so the vias are tented. The problem seems to occur due to the relative closeness of some via holes to the BGA pads. On another revision of the PCB, I will pull the vias further away from the pads. Thank you very much for the link to the fine wire.

glitch: That is a great piece of advice. I will try pushing fine wire through the via hole, and I will also try heating the BGA with a hot air station. I have access to a Hakko FR-830 pre-heater and a Hakko FR-802 hot air gun. Unfortunately, I don't have any fancy vision placement system, but that shouldn't be a problem.

Just to be certain that I don't "cook" the PCB during the rework process: what should be the maximum temperature of the pre-heater and the hot air?

dksmall

Level: Raving Lunatic

Joined: Mon. Apr 16, 2001

Posts: 3676 View posts

Location: Phoenix, Arizona

Posted by dksmall: Tue. Mar 22, 2011 - 03:34 PM

This is why I brought the DRC issue. Our Mentor guys have rules in place that don't allow un-tented vias under parts (so contaminants won't get trapped under the part). And now with BGA parts I think they restrict the use of via's under the BGA part.

nkinar

Level: Hangaround

Joined: Wed. Jul 18, 2007

Posts: 399 View posts

Location: Canada

#10

Posted by nkinar: Tue. Mar 22, 2011 - 04:02 PM

dksmall: Thanks for pointing this out. I think that Altium Designer doesn't automatically enforce distances of vias to pads; I would have to set up this rule myself. On the other hand, I think that this design rule is automatically enforced by Eagle without any setup. Yes - the design rules are extremely important.

ignoramus

Level: Raving Lunatic

Joined: Sun. Aug 4, 2002

Posts: 2140 View posts

Location: Brisbane, Australia

#11

Posted by ignoramus: Tue. Mar 22, 2011 - 09:30 PM

Altium does have a clearance rule setting which will ensure the minimum distances between various types of features.

The designer needs to define these parameters.

nkinar

Level: Hangaround

Joined: Wed. Jul 18, 2007

Posts: 399 View posts

Location: Canada

#12

Posted by nkinar: Tue. Mar 22, 2011 - 10:01 PM

Thanks for pointing this out, ignoramus; I suppose that I have to be very careful when setting the design rules up. Having used Eagle CAD for many years, I find that Altium is a little bit different: there is indeed a learning curve.

I tried stripping a stranded wire and then inserting one of the wire strands into the via. I attempted to warm up the wire with hot air. For me, this didn't work since the wire "buckled" and refused to enter the via, due to the solder already in the hole. Despite all of my trying, I couldn't push the wire into the hole.

I then removed the decoupling capacitors from the bottom of the PCB. These capacitors are placed on the bottom of the PCB to provide decoupling for the microcontroller power rails.

I placed the circuit board right-side up over a Hakko FR-830 preheater and tried to use hot air produced by the Hakko FR-802 soldering station to "bump" the BGA, as recommended in this thread.

However, I think that a much larger nozzle would be required to cover the entire BGA.

I found that the BGA refused to move, presumably because hot air was not being applied over a much larger area. The maximum temperature being applied to the part was 300 deg Celcius.

What might be needed here is a rework station for BGAs.

nkinar

Level: Hangaround

Joined: Wed. Jul 18, 2007

Posts: 399 View posts

Location: Canada

#13

Posted by nkinar: Wed. Mar 23, 2011 - 05:23 AM

In the event that my clumsy hands are unable to perform the rework outlined in this thread, could anyone suggest a company that would be able to rework and then inspect my circuit board? Preferably the company would be in Canada.

What would be the turn time for such rework? Would it be possible to get this stuff taken care of in only a few days?

meslomp

Level: Raving Lunatic

Joined: Wed. May 2, 2007

Posts: 5714 View posts

Location: Nieuwegein, Netherlands

#14

Posted by meslomp: Wed. Mar 23, 2011 - 06:25 AM

I do not know in canada, but you could do a search on pcb board assemblers. Then find one that does BGA soldering. They should then also have an inspecion facility.

nkinar

Level: Hangaround

Joined: Wed. Jul 18, 2007

Posts: 399 View posts

Location: Canada

#15

Posted by nkinar: Wed. Mar 23, 2011 - 01:57 PM

Thanks for the response, meslomp. I will try to locate a pcb board assembler that might be able to help me. However, I would like to find someone that is able to successfully do such rework.

I've attempted to search around Canada in the past, and I've found it somewhat difficult to find someone who has both the facilities and the expertise to both work with and repair BGA parts

meslomp

Level: Raving Lunatic

Joined: Wed. May 2, 2007

Posts: 5714 View posts

Location: Nieuwegein, Netherlands

#16

Posted by meslomp: Wed. Mar 23, 2011 - 03:45 PM

how far in the past is that?

note that BGA's have become immense popular last years, so a board assembler that did not have the stuff a couple of years ago could have had to buy the parts needed to do BGA placement and inspection, they then probably also have a rework station as they need to be able to repair the faulty PCB's .
I heard on a seminar over here a while ago (from pultiple assemblers)that most of them also seem to be able to re-ball (place new balls on the BGA) BGA's so it might not even cost you a BGA ( dont know the cost though).

did a search on "canada pcb assembler" and saw a number of links that look interesting.

regards

nkinar

Level: Hangaround

Joined: Wed. Jul 18, 2007

Posts: 399 View posts

Location: Canada

#17

Posted by nkinar: Thu. Mar 24, 2011 - 08:07 PM

I've made some phone calls, but I am finding that the companies I phone are not very willing to do this type of rework. They generally want to assemble full circuit boards.

In the event that I cannot find anyone to do this type of rework locally, could anyone suggest the name of any company that could help me out?

Once again, I have a problem where a few vias (less than 10 per BGA) are placed close to holes. Only one via is situated in a pad.

I would prefer to salvage the prototypes that have been created. With the proper equipment, it shouldn't be too difficult to either perform the rework mentioned in this thread or to do something else.

Alternately, the BGAs could be removed, and the via holes could be covered with soldermask paint. Moreover, the vias could be covered over with tiny bits of copper trace rework material.

I can imagine doing this myself, but I do not have access to a BGA vision placement system so that the BGA parts could be placed back on the circuit board. Note that the circuit board is semi-populated, so I might not be able to place it through a reflow oven again. There are also parts placed on both sides of the PCB.

glitch

Level: Raving Lunatic

Joined: Sat. Jan 12, 2002

Posts: 8696 View posts

Location: Canada

#18

Posted by glitch: Thu. Mar 24, 2011 - 08:28 PM

you don't need a vision system, only a proper rework station that can heat he board and part properly. Sounds like what you have access to gets you half way there, all you need is a proper heater for the top-side. [my apologies, as you earlier said "hot air gun" so I thought you had the right stuff - did not look up the part... what you have is a "hot air pencil", which is insufficient for BGA rework. - except maybe for a really small package]

Writing code is like having sex.... make one little mistake, and you're supporting it for life.

nkinar

Level: Hangaround

Joined: Wed. Jul 18, 2007

Posts: 399 View posts

Location: Canada

#19

Posted by nkinar: Thu. Mar 24, 2011 - 09:58 PM

Thanks, glitch. Yes, I now wish that a proper rework station would immediately appear in front of me so that I can get this job done ;-)

I now have managed to locate a syringe with an extremely small diameter. (Borrowed from a research lab in another department.) The syringe is small enough to fit into the via hole.

I am thinking that it might be possible to fill the syringe with solder paste, and then squeeze the solder paste into the via hole.

Heating the via hole with my hot air pencil might cause the solder paste to liquify. I will try this and then post back my results here.

tpappano

Level: Raving Lunatic

Joined: Mon. Dec 1, 2003

Posts: 2937 View posts

#20

Posted by tpappano: Fri. Mar 25, 2011 - 12:37 AM

I accidentally barbecued a TSSOP with a bottom side ground pad. Not wanting to throw away my new sample board and not having any "rework" tools, I ground the part completely off the board with a Dremel tool, then reflowed a new part by applying my *big* iron to the underside of the board. It lives. This could be a little dicey with a BGA...

Tom Pappano
Tulsa, Oklahoma

gchapman

Level: 10k+ Postman

Joined: Tue. Jan 9, 2007

Posts: 10514 View posts

Location: Arlington, Texas, u.S.A.

#21

Posted by gchapman: Fri. Mar 25, 2011 - 01:21 AM

A tech told me he re-works BGAs with a heat gun!
So heat gun, PCB pre-heating (heater, griddle, or second heat gun), and some protection for other parts.
For parts protection, one way is JBC Extractors and protectors.
Or, simply use aluminum foil.

"Dare to be naïve." - Buckminster Fuller

gchapman

Level: 10k+ Postman

Joined: Tue. Jan 9, 2007

Posts: 10514 View posts

Location: Arlington, Texas, u.S.A.

#22

Posted by gchapman: Fri. Mar 25, 2011 - 01:40 AM

via fill - I'd use solder paste and a squeegee (solder paste does not flow well).
Heating the via hole - similar to what's done with SchmartBoard's BGA products; I guess they use micro-vias.

"Dare to be naïve." - Buckminster Fuller

nkinar

Level: Hangaround

Joined: Wed. Jul 18, 2007

Posts: 399 View posts

Location: Canada

#23

Posted by nkinar: Fri. Mar 25, 2011 - 03:23 AM

You guys are absolutely great. Thank you very, very much gchapman and the rest of the people who responded to this thread! (LOL, I also like the idea of tpappano with the Dremmel tool; I just purchased one of these a few weeks ago and I am still learning how to use it.)

The BGA solder pad is now fully connected, and after running a test program on the SDRAM memory bus, I am happy to say that it appears to work well. Here are the steps that I took:

(1) I inserted the needle of a tiny "diabetic" syringe into the via hole. Applying heat at 300 deg Celsius with my Hakko FR-802 soldering pencil (and using a small-diameter nozzle), I depressed the plunger of the needle in an attempt to push the solder down the via hole. The syringe was filled with nothing more than air, and the FR-830 preheater was set at 150 deg Celsius. Looking at the board under a magnifier, I noticed that the solder ball in the via went a little ways down the via hole, but the test program showed that this procedure did not work to fully connect the BGA pad.

(2) As suggested by gchapman, I looked at how the SchmartBoard products work. I spread a tacky no-clean flux over the via area (ChipQuik SMD291NL). Then, as shown in a YouTube promotional video for the SchmartBoard products (http://www.youtube.com/watch?v=D...), I spread solder over the via using an OK International PS-900 soldering iron.

(3) I then cleaned the via area with Isopropyl alcohol and Kimwipes. Some tacky flux remained in the via hole. Using the FR-802 and FR-830, I preheated the board to 150 degrees Celcius and used the soldering pencil to warm the via area to a temperature of 300 deg Celsius (using a small-diameter nozzle). I suspect that the tacky flux helped to conduct heat into the via.

This connected the pad. I suspect that steps (2) and (3) worked the best in this procedure.

Such a situation strongly reminds me that the art of engineering is more than just making things work; we also need to deal with the unusual cases that make this endeavor equally frustrating and extremely rewarding. This is a thread that I will indeed print out and keep in my ring binder of "solutions".

So once again, thank you very much to the people who responded to this thread - this certainly made my day, and I hope that good karma flows to all of you as well :-)

Many thanks.

gchapman

Level: 10k+ Postman

Joined: Tue. Jan 9, 2007

Posts: 10514 View posts

Location: Arlington, Texas, u.S.A.

#24

Posted by gchapman: Fri. Mar 25, 2011 - 07:14 AM

Alternate prototyping method:
If one has the room and power, ideally all BGA parts are on an off-the-shelf CPU (MCU, RAM, Flash);
then, one's custom circuit is on a PCB that mates with the CPU.
Sometimes the custom PCB is an inexpensive 2-layer.

ARM9:
Fyi, there are a few that come in QFP in addition to BGA. One is Freescale i.MX233; an i.MX233 CPU is Chumby Hacker.

Dispensing:
By hand this can be difficult with fluids that are not viscous enough (like soldering paste).
There are differences in soldering paste w.r.t. dispensing; this is by adjusting the paste's volume ratio of flux to solder balls.
Some pastes are for stencil printing and others are for rework (dispensing).
Its much easier to use a pneumatic dispenser versus a syringe for some fluids.
If not using soldering stencils a lot and doing a lot of re-work, consider acquiring a dispenser.

Flux:
There are BGA-specific fluxes. Apparently some fluxes sputter too much which could cause a no joint, bad joint, or a mis-shapen joint (a stress riser).

300 deg. C:
Careful; usually don't need that high a temperature even with lead-free. If linger too long at that temperature, PCB could start to de-laminate, pad lifts due to loss of adhesion of glue between pad copper and PCB, or crack a via. A good thing about PCB pre-heating is the additional heat (by soldering iron, or, hot air) can be limited. If damage occurs, there are some companies that make PCB repair kits (epoxy, glue for pads, via replating/conductive paste).

nkinar wrote:

I suspect that the tacky flux helped to conduct heat into the via.

True but will get much greater conduction via melted solder. Flux does remove oxides so that the solder can flow. Can apply the tacky flux, drop BGA, align BGA, pre-heat PCB, heat gun the BGA. But usual method is soldering paste; there are BGA-specific mini-stencils used for BGA re-work and BGA re-balling.

nkinar wrote:

Such a situation strongly reminds me that the art of engineering is more than just making things work; we also need to deal with the unusual cases that make this endeavor equally frustrating and extremely rewarding.

One usually doesn't learn that art in engineering school; that's a problem because one needs that art.
Recommend replacing a few topics in an engineering school lab with some prototyping hands-on.
Else, its jump into the pool's deep end out in the work world.
Sometimes art is learned out of necessity due to not enough people (no technician therefore you also do the tech work).
Too much thinking and not enough tinkering ;-)

"Dare to be naïve." - Buckminster Fuller

nkinar

Level: Hangaround

Joined: Wed. Jul 18, 2007

Posts: 399 View posts

Location: Canada

#25

Posted by nkinar: Fri. Mar 25, 2011 - 02:50 PM

Great advice - thank you again; this is much appreciated! :-)

bigsmooth

Level: Hangaround

Joined: Fri. Sep 29, 2006

Posts: 307 View posts

#26

Posted by bigsmooth: Tue. Sep 4, 2012 - 03:34 AM

Any chance you could post the eagle files for the BGA package? I can't seem to find one.

nkinar

Level: Hangaround

Joined: Wed. Jul 18, 2007

Posts: 399 View posts

Location: Canada

#27

Posted by nkinar: Tue. Sep 4, 2012 - 02:49 PM

I actually used Altium for this design, but I've used Eagle in the past. I think that there's a script in Eagle that you can use to generate the BGA package. I actually ended up making a revision of this circuit board and covering the vias with soldermask to ensure that the solder balls do not fall down the holes. I also shifted some of the vias away from the via holes.

bigsmooth

Level: Hangaround

Joined: Fri. Sep 29, 2006

Posts: 307 View posts

#28

Posted by bigsmooth: Tue. Sep 4, 2012 - 02:52 PM

nkinar wrote:

I actually used Altium for this design, but I've used Eagle in the past. I think that there's a script in Eagle that you can use to generate the BGA package. I actually ended up making a revision of this circuit board and covering the vias with soldermask to ensure that the solder balls do not fall down the holes. I also shifted some of the vias away from the via holes.

Could you please post a screen shot of your escape routing? I've never done this, so I'm trying to see examples.