0.65mm BGA / JLCPCB / Hot Air! - Page 1
Forum section: electronics / projects

author: essele
author_rank: Frequent Contributor
timestamp: April 01, 2021, 10:06:37 am
content: I've been experimenting with a PSoC 6 which is only available in horrible packages, and I struggled to find much online about how to work with BGA's as a hobbyist, so I thought I'd post my exploits which may help others, and hopefully improve what I'm doing.The most helpful post I found was this one:https://www.eevblog.com/forum/projects/0-65mm-bga-rules-suggestions/... although it seemed like a bit of a battle with JLC. I did drop them a note with some sample gerbers to ask about capabilities for BGA, but I'm impatient so pressed ahead and submitted a design anyway (they did later reply saying they could meet my required capabilities.)I actually found this NXP article to be the most helpful in terms of track widths and via sizes:https://www.nxp.com/docs/en/application-note/AN10778.pdfThe device I'm using is a Cypress (now Infineon) PSoC 6 in a 124 ball 0.65mm pitch package. I decided to build a test board that breaks out every IO pin on the device so that I can easily test if each pin is connected.So I am using KiCad, with 5mil tracks (with 4.8mil/0.122mm clearance for DRC), and 0.425mm Vias with a 0.2mm hole (as per the NXP doc.) I kept it simple, placed the via's equidistant between the pads (I assume you could move them closer to the connected pad to get a greater clearance.)Obviously to meet these specs (with JLC) you need to be using a 4-layer board, which is a shame because (if you don't have full utilisation) I'm pretty sure you could handle the PSoC routing on a 2-layer ... although small 4-Layer boards aren't actually that expensive now! Technically the 0.425mm via is below the 0.45mm limit which imposes a 4-wire kelvin test ... but that's a button you have to click, so I decided to try my luck and not click it (it adds about $30 to the cost.)I also put some alignment marks on the board, but in copper to improve accuracy compared to the silk screen. Also following another tip I made sure there was a pin1 marker outside of the footprint, so it can be seen with the device mounted.There seemed to be no issue with the order, no questions, and the board was put into production ... and a relatively small number of days later they arrived, looking amazing (at least to me as a BGA virgin!)BGA SOLDERING ATTEMPT #1:I've never really got into the stencil and solder paste side of things, I prefer hand soldering and use the JLCPCBA service when things get a bit tedious ... and I'd like to use these devices on a board where most of the rest of the components are handled by PBCA, so the BGA needs to be added later, therefore a stencil isn't going to work.So for my first attempt I smeared a thin layer of flux (the gel kind) over the footprint on the board, mounted the BGA (which did seem to "fit" and stay in place) and used one of the nifty USB hotplate devices to heat up the middle of the board. I had an IR thermometer checking the temperature of the top of the BGA and wanted to take it up to about 260 degreesC.The IR thermometer was a bit all over the place, not sure if this is the device or some issue with emissivity and the hotplate was at 300 degrees for some time before I got a level of confidence it had reflowed. With hindsight I think this was way too much, the board was discoloured slightly on the bottom, but it did all appear to have flowed, you could see the balls around the edge of the device and things looked good.So I soldered on my programming connector and connected the programmer to see if the device could be detected ... nope! Power was there, and a quick check on some of the breakout pins showed a non-open, so it seemed like some things were ok, but it wasn't working. (See later, I'm way too impatient, I actually think it was soldered ok at this point!)In an attempt to fix it I decided to apply some flux and hot air and push it down a little ... this was a stupid thing to do. I was a bit heavy handed in testing (gently pushing on one side and seeing if it comes back to the right place) and pushed it too far, so I had to move it back ... it seemed to align ok and I pushed it down with my tweezers before removing the heat.It also didn't work, and I now had a power to GND short, so clearly I had some bridges under the chip. So I removed it and yes there were three areas where the balls had joined together. Chalk attempt 1 up to experience and move on!BGA SOLDERING ATTEMPT #2:This time I decided to go straight for hot air ... and also used an appropriately sized nozzle. So a new board, a new chip, some new flux thinly smeared on the footprint as per the above.I use a mains powered hot air gun (I think it was from Ali, but I've had it for years and use it all the time) mainly because I don't have the space for a desk based one. I had it set to 320 degreesC and a relatively high airflow because of the larger nozzle than usual.After about 2 minutes I "tested" and the chip moved very slightly and then sprung back to the right position so it seemed to be ok. I gave it another 10 seconds and then removed the heat.Again, soldered in the debug connector, and ... nope! Not detected. I tried a different programmer, still not working.So this time I was a bit more methodical ... I soldered in some of the decoupling caps, and the linear regulator cap for the IC just in case they were the problem (they weren't), and then started testing. The linear regulator was generating the 1.1V for the core, so that was at least connected along with power. I then had a quick look at all the breakout pins.Every single pin was connected (non-open to GND) ... so whilst I was always suspecting the BGA soldering I couldn't understand how 100+ pins were all fine, but the one or two critical pins that were needed to power the device weren't connected??? After some more checking of pinouts (I've been caught by bad library symbols before) I finally discovered that I had swapped the clk and data lines for the debugger! A quick bodge later and it worked!So at this point I suspect that the first attempt would have worked also, although the temperature profile for this needs to be looked at to stop the board discolouring, and I actually found the hot-air approach to be surprisingly straightforward so I will probably stick with this.I have a few more boards/devices to experiment with before I move onto designing this into a proper device, but at initial go, this is pretty simple ... you can get low cost 4-layer boards that meet the needs for 0.65mm pitch BGA's, and you can hand solder them with nothing more than hot-air. I'm super excited as it opens up a much wider set of possibilities.I've attached an image of the relevant bit of my layout, and a closeup of the BGA footprint on the delivered boards, along with a couple of photos of the board.I hope this is helpful for anyone else considering or battling with BGA's, and I'm very keen to hear if there are things I could do to make it even easier.Lee.

author: moffy
author_rank: Super Contributor
timestamp: April 02, 2021, 07:24:11 am
content: Thanks for the info, this is both interesting and valuable for the electronics hobbyist.

author: ali_asadzadeh
author_rank: Super Contributor
timestamp: April 02, 2021, 07:48:27 am
content: Thanks for sharing, your BGA is not fully Grid, so maybe that's why they make it at JLCPCB, because if you add more pads inside the BGA, your traces would have to pass near vias, and since it's under 0.127mm they would reject it.so you choose 4.8mil for trace and 0.122mm for clearance and a 0.425mm via with a 0.2mm whole size?Have you tired a fully populated BGA chip?

author: essele
author_rank: Frequent Contributor
timestamp: April 03, 2021, 05:31:58 pm
content: Hi ali_asadzadeh,Yes, I hadn't actually thought too much about running tracks between the vias as it was not needed for my use case -- so you are correct, I doubt very much you could get too far with a full grid BGA, I guess it would depend how many of the pads you needed to use.I'm using 5mil tracks with 1.22mm clearance, and 0.425mm via with 0.2mm holes ... if you add up up all the bits including pad diameter, clearances, and via dimensions you'll see that these are the maximums you can get away with in a 0.65mm pitch ... you can't quite do 5mil clearance ... but JLC is 3.5mil track/clearance anyway, so you could probably vary things a bit.

author: Mecanix
author_rank: Frequent Contributor
timestamp: April 03, 2021, 07:34:04 pm
content: 1) I normally flux the pads, apply a dab of fresh solder paste onto the tip of my iron, and freshen those bga pads on the pcb leaving as much solder as those tiny pads can take(to ensure evenness).2) I do the same as step1 but on the bga IC pads (grandma's Top Secret tip!)3) Clean-up everything >> add flux again >> place bga IC >> hot air in one hand, tweezers in the other >> everything snaps in place like a LEGO block, every time!Kudos to JLC, they certainly get the job done.

author: essele
author_rank: Frequent Contributor
timestamp: April 03, 2021, 07:58:48 pm
content: Hi Mechanix,Doesn’t step 2 destroy the balls?With my first attempt I obviously wrecked things, so I have bought some 0.4mm balls to experiment with reballing (since I’ve never tried), but I don’t see how running an iron over the BGA or is ever going to make things better?

author: Mecanix
author_rank: Frequent Contributor
timestamp: April 03, 2021, 08:16:49 pm
content: I'd guess; if you know that your bga chip is fresh i.e. just out of the foundry, then probably okay to skip that step.If old and oxidized like the ones I need to work with, then its probably not a bad idea to submerge those bad boys into flux, swipe them quickly with fresh solder and re-sphere them up a bit.Can't vouch saying it does a better sphere than factory but the technique certainly brings the yield up to 99% in my case... which is what I'm mostly interested in.

author: SilverSolder
author_rank: Super Contributor
timestamp: April 03, 2021, 08:53:56 pm
content: Quote from: Mecanix on April 03, 2021, 08:16:49 pmI guess the fact that you pre-tin both the chip and the pads is what makes this work? As long as the "sum of the solder" between the two approaches a ball size, and is evenly distributed, it seems like a pretty cool technique...

author: Mecanix
author_rank: Frequent Contributor
timestamp: April 03, 2021, 09:18:41 pm
content: Can't take the credit on the technique, it was given to me by someone back when I was really struggling with some 3x3 0.5mm pitch QFN package (bringing-a-lot). Only when refreshed with new stuff all over they ended up snapping like lego blocks each and every time, literally. *no thick paste/stencil games*, just pre-tined 'generously & evenly' on both the PCB and the IC.Then came those even nastier bga yielding as low as 50% on the benchtop here :/ Total frustration, had'em bridged, NC, was all over. Technique above worked equally well for theseQuote from: SilverSolder on April 03, 2021, 08:53:56 pmCan't accurately measure if the solder is the same amount as when factory ball'ed, probably a tad less in fact. I'll soon have another batch of 20x to hot air in a month or two, let's see if I can remember to take some HD pics and upload here.

author: ali_asadzadeh
author_rank: Super Contributor
timestamp: April 04, 2021, 05:46:47 am
content: Mecanix thanks or sharing the info, if you could also make some videos, that would be supper cool

author: voltsandjolts
author_rank: Unknown
timestamp: April 04, 2021, 09:38:35 am
content: The pre-tinning PCB and IC trick makes it tempting to try DIY via-in-pad. Just fill the vias yourself when tinning the footprint.For low volume self-build it could enable narrow pitch on cheap PCB process. 0.2mm via holes ain't gonna wick much after a solder pre-fill.

author: Mecanix
author_rank: Frequent Contributor
timestamp: April 04, 2021, 06:54:06 pm
content: Quote from: voltsandjolts on April 04, 2021, 09:38:35 amlol if that works out it is sure to send some fancy fab houses into reconsidering their pricing list. Has to be "illegal"Seriously though, you've just shared a great idea right there. I'll give that a shot on a 4-layer test board with a cheap bga, let's see...

author: Yansi
author_rank: Super Contributor
timestamp: April 04, 2021, 08:13:30 pm
content: Awwww good on you that it all worked out!I am still a BGA virgin and need to learn to solder those suckers. A lot of the stuff I'd like to play with comes of course in BGA only packages, as is the norm these days.

author: julian1
author_rank: Frequent Contributor
timestamp: April 04, 2021, 09:15:09 pm
content: Quote from: Mecanix on April 03, 2021, 07:34:04 pmI wonder if this approach would also work for tqfp. Just bead the pads up on the pcb. apply lots of flux. Then drop the part on and heat with a hot air gun.I find controlling solder paste volume is hard without a stencil.

author: essele
author_rank: Frequent Contributor
timestamp: April 08, 2021, 04:11:20 pm
content: Just a little update ... I took the chip from my unsuccessful first attempt, removed it, cleaned off all of the balls, and manually reballed it using 0.4mm (leaded) balls from eBay, a tiny amount of flux and some very slow hot air.I soldered it to a new board and it works perfectly! All pins connected, and detected by the debugger.I'd like to say I only reballed it once, but unfortunately I soldered it in place upside down the first time (doh!), so I had to do it twice. It's strangely relaxing, and really quite a good experience to watch them all line up nicely with a bit of hot air (well, most of them anyway!)So I feel like I've made giant leaps over the last week ... I've proved to myself that BGA's are absolutely doable and not scary, and even if you mess them up, you can reball and try again! (Albeit with a relatively small device.)

author: maxkunes
author_rank: Newbie
timestamp: April 09, 2021, 05:35:07 am
content: For a project at work, I've been placing quite a few boards with .6mm pin pitch 200+ ball BGAs. I've also done some terrible .4 mm (probably less) ball pitch packages where the chip is only about 1mm wide. However, the tips below make that not too difficult either.I have two recommendations:The solder paste and oven characterization make a bigger deal than I imagined. We have now properly characterized our conveyer oven and switched to GC10 (with the smallest particle size) and we have had pretty much 100% success over 20 or so boards. Not a single board had a BGA short, I think I got a couple too hot though.Compare this to a smaller in early 2020 with some MG chemicals paste, most of the boards I made had a short under the BGA once out of the oven.However, I've had very good success air-gunning small pin pitch BGAs. Just brush a small layer of good Amtech flux on the clean ball pads (if you put too much the chip will jump around due to the boiling flux) and use pretty much any temp you want (for efficiency I usually just use high temp + high air). Once you see the chip move a little, you can fairly aggressively knock it around with tweezers to ensure it sat in place properly.

author: Mecanix
author_rank: Frequent Contributor
timestamp: April 09, 2021, 05:47:51 am
content: Quote from: julian1 on April 04, 2021, 09:15:09 pmPersonally for tqfp I'm utilizing the 'drag' method from J.Gammell. You'll bridge a few pins practicing and while getting used to your hardware however on your third or fourth attempt (and beyond) it takes <15secs once you get used to it. Never stencil my tqfp anymore probably for the same reason you have (occasional bridging, rework reqs, misalignments, joints strength, potential overheating, etc etc).

author: SilverSolder
author_rank: Super Contributor
timestamp: April 09, 2021, 12:46:07 pm
content: Quote from: Mecanix on April 09, 2021, 05:47:51 amNotice how little flux he applies in the video? It doesn't take so much. - I cringe whenever I see videos where the whole PCB appears to be submerged in 1/2 inch of flux...