-
PIC16F18856 seems to be having problems with dry joints.......~5% of boards
Posted by ocset on 11 Apr, 2018 05:26 -
Hello,
Our PCB assembler have told us that they are getting difficulties with soldering the PIC16F18856 [28 pin UQFN (4x4) ] on our board.
They have actually asked us to make the copper pads smaller so that a solder resist bridge can be layed down between the pads. However, we are already using the microchip recommended footprint. (page 657 of datasheet)
Anyway, we are also getting problems with the lamp product that the micro is in. We configure the micro at production time so it knows what maximum dimming level to be at etc. Problem is, sometimes, (say in 5% of cases), the lamp doesn’t actually come back on after its startup routine. (the startup routine involves, whenever the lamp is switched on, the lamp comes on for 1 second, then dims down for 1 second, then goes off, then comes back on again, -just so’s we can see that the micro is compus mentus)….however, in say 10% of cases, the lamp doesn’t come back on after being configured.
We suspect this is due to dry joints in the micro pads. –eg the micro pin that connects to the light sensor may be dry and it may be seeing noise and think its light when its actually dark. Or the pin that connects to the temp sensor may have similar issues and think its too hot to turn the lamp back on etc etc.
Do you have any tips on ensuring no dry joints with this kind of footprint?
Our footprint is exactly as on page 657 of the datasheet, but the assemblers want the pads trimmed back so solder resist can go between the pads……we currently have a 0.1mm solder resist bridge between each pad on the gerbers , but its so thin that the PCB manufacturer can’t produce it, and so we have no solder resist between the pads…the PCB assembler is complaining about this and reporting many failed boards to us.
PIC16F18856 datasheet
https://www.microchip.com/wwwproducts/en/PIC16F18856
(page 657 shows footprint of 28 pin UQFN)
We are also wondering about buying a cheap reflow oven so we can remove and resolder the micro ourselves so as to try and repair potential dry joints.
Do you know of a cheap reflow oven.?
(The boards are 10cm by 8cm and 4 layer, components and leds only on top.)
-
I don't think that making the pads smaller will help. You would do that if you get shorts between pins.
What you likely have issues with is the pads being corroded due to improper storage of the chips or the temperature profile of there reflow oven is not hot enough (That can happen if you have large internal copper pours or large heavy components close by).
The solder paste also makes a big difference. Old paste can have bad performance. Also all pastes are different, some have better flux in them and that can make a massive difference on hard to solder parts.
As for fixing these you can just run a soldering iron with a small tip around the QFN chip to reflow the pads, adding some liquid flux before soldering also helps a lot. If you want to replace the chips its best to just get a cheap chinese hot air station to heat up just the part of the board where the chip is and pick it off with tweezers, same procedure in reverse for putting a new chip down. -
For in-house rework, hot air should be adequate.
As regards product problems, you need to add soem diagnostics to teh code so you know what's happenning.
-
If your assembly shop is reasonable they should have a small x-ray that helps them pinpoint these issues. We've had these type of issues with BGA's and things like POP memory. I'm not sure you should be having it on a part like that.
-
Shoddy contractors strike again. Isn't this the bane of your life, treez? They're either using bad solder paste, or have left chips/boards out in the open for too long.
Of course, it doesn't help that you've picked a 0.4mm pitch QFN... if you're redoing the boards, consider switching from the 4x4 0.4mm QFN to the 6x6 0.65mm QFN.
Rework: As other have said, hot air. Put a generous amount of flux around the chip, heat it up until the solder is molten, and gently tap it/push it around slightly, and watch it snap back in position. If it's not properly centered, do so. You may find a microscope or some other form of magnification helpful.
Just re-heating the boards in an oven is not a magical fix, especially if you don't add any flux to them. -
Did you really need such a small package? Fine-pitch QFNs are bitches. Assemblers hate them. Only a very few PCB manufacturers would be able to put solder mask between the pads at this pitch. And yes, without solder mask, the probability of solder bridges on such packages is huge.
Modifying pads, solder paste mask, etc, is a possibility but pretty much trial and error and would cost you a fortune in time (and money) until you get it right. There's no absolute "right" either, it's all a matter of what both your assembler and PCB manufacturer can do.
In-house "post-processing" reflow? You're in for a continous stream of pain if you go that route for production. Believe me. And your second reflow may also cause other problems. Your PCB may not like that very much. Did you select a high-TG PCB? -
With that pitch, I would need to manufacture PCB with such a grade that 5 mil drill hole sizes are supported with 2 mil trace/space, and use only gold ENIG finish, with no heavy copper finish otherwise the IC may not sit perfectly. As for the paste stencils, I would only use high end stepped stencils which are 500$-2K$ stencils which have multiple thicknesses around different pad sizes to allow different levels of paste on different size & pitched pads of different sized components to optimize soldering with the right amount of solder paste at different areas. Any lower quality range PCB and stencil, I would not use such a fine pitch component.
-
As Brian said, PCB finish/planarity are key facts when dealing with those fine-pitch QFNs. The problem is that they lay flat on a large surface and thus are much less forgiving than BGAs. Most assemblers I've worked with told me they much prefer dealing with BGAs than QFNs in general.
The fact that your assembler suggested shrinking pads so as to get solder mask between pads most likely tells that they add issues with solder bridges or at least they were expecting to. So that's very possible that they shrunk the solder paste mask's openings to reduce the amount of solder paste on those pads so as to reduce the probability of solder bridges. But by doing so, the quality of solder joints was compromised (probably due to planarity defaults).
So - to get more advice, please tell us what class of PCB you chose and what kind of finish, also the TG if you have that.
Of course for this kind of device - which I doubt is THAT miniaturized - you should go for larger-pitch packages.
Additionally, if I got it right, you get issues with like 5% of your boards (is that right?). I'm really not sure it would be worth the trouble of reworking those boards instead of trashing them. Just estimate the costs. Still, I would be wary of reliability on boards that *seem* to work fine, so you should get this assembling issue fixed anyway.
-
It gets even worse if these components are in street lights which will bake in the sun every day in summer and freeze back and forth in the winter, or if the component is potted, things will get worse. With such a small fine pitch device, with these temperature stresses, the microscopic solder joints will snap within a year under such conditions. Faster if there is a weak but functional joint.
Functional at test bench isn't enough. You must take into consideration environmental stresses over time unless you are not interested in providing warranties.
-
Thanks, i was wondering if Microchip meant it for use only with leaded solder?
I realise that leaded solder gives far batter quality joints with such small pitch chips.
We might be able to ship these boards to our Customers in non-ROHS countires.
Incidentally, attached is the gerber showing top copper (red) and top resist (pink)....also shown is a sot23 elsewhere on the same board...it looks well depleted of solder, and all the components have this sparsely soldered appearance.
-
Quote
The fact that your assembler suggested shrinking pads so as to get solder mask between pads most likely tells that they add issues with solder bridges or at least they were expecting to
Thanks, yes we did, on the first batch of these boards we had pretty few failures on this same pic16f18856 footprint, , but all failures were pins soldered together, and we could see the offending shorting solder.
I think as you suggest, they may have limited the solder to stop these shorts, but they perhaps went too far, and now we have a significant number of faulted boards, and we are not sending any of this large batch out.
But as many kindly point out here, this UQFN footpring (0.4mm pitch) seems like a bad thing. I really think we will have to step up to the 6X6mmQFN part on the next board...we may just be able to squeeze that on.
Woudl be nice if we could find som way of using these non-populated boards though......we are scared to send them for assembly after this last batch.
Maybe doing them with leaded solder and sending them to our African (eg non European) customers?
I am wondering if we can risk getting another batch assembled, and tell the assembler to use much more solder, and then some boards will get pic16f18856 shorts, (and we'll have to just scrap those) but thats gotta be better than dry joints which may emerge say a year later in the field.? The other alternative is just to bin all these great many unpopulated boards...because of this horrible pic16f18856 footprint. I am surprised Microchip didnt put a note in the datasheet about this UQFN 4x4mm part, and its difficulty in soldering.
I will find out what TG rating the FR4 has to be, our boss knows......do you know what TG rating the FR4 has to be for soldering these UQFN (4mm pitch) parts? -
Some assemblers can work just fine with 0.4mm pitch QFN with the footprint from the datasheet and others can't. I got the strong recommendation to keep at least 0.2mm between the pads and thus leaving the pads 0.2mm wide to prevent bridging (no matter what the footprint in the datasheet says). Also I wouldn't keep the pads very small. I always make the pads stick out under QFN device because like a nice heel at the base of the QFN so I can make sure the solder has flow properly c.q. the flux did it's job. If the assembler screws that up it is on them; they have to adjust the profile of the oven properly.