Please recomend PCB fab for fine pitch BGAs?  - Page 1
Forum section: electronics / general

author: David Chamberlain
author_rank: Frequent Contributor
timestamp: April 29, 2018, 07:49:59 am
content: I'm trying to get a PCB fabricated where the smallest pitch component is a WLCS BGA 0.4mm pitch with recommended landing pad NSMD 0.21mm. My usual go-to fab (who's name I will not mention because they don't require any more free advertising) said (via email) they can do 0.1mm via drills and via-in-pad. I'm a little nervous because the 0.1mm drill is slightly smaller then the advertised minimum of 4mil so am guessing they might just drill at 4mil.So anyway, my actual question is has anyone here used / can recommend an economic pcb fab that can do the following...If not via-in-pad then I am currently able to route the board with a min clearance of 0.1mm with uVia diameter 0.15mm, 0.1mm drill and min trace width of 0.127mm. If I do all that then overall I am able to achieve 0.1mm clearance all around.If I were to do via-in-pad then I could increase my clearance but not having done it before I'm worried about other issue such as reliability especially if the board are being made down to a cost. In that case I would prefer to stick with the dog bones above.Thanks[edit: removed 'Chinese' from title as it's not particularly relevant except to imply low cost]

author: Harjit
author_rank: Regular Contributor
timestamp: October 02, 2021, 02:54:59 pm
content: What did you end up doing? How did it turn out? I've got a 0.4mm BGA that I need to work with. Thanks.

author: mon2
author_rank: Frequent Contributor
timestamp: October 02, 2021, 03:13:11 pm
content: Hi Harjit. We are working with WLCSP devices with 0.4mm pitch balls. Is your PCB layout demanding via-in-pad support ?If yes, then you are into HDI PCBs and they can be $$$. We recently scouted around for suppliers (offshore) and found varying results from 'unable to do it' to typically $1200 USD - $1800 USD for 30 pcs of our PCB (prototype run). Could not believe the PCBs to be so costly and our spidey-sense was correct. This exercise is all about finding a shop who considers the HDI process as a 'normal' PCB rather than a premium process. Would not doubt that some just run across the street to another PCB shop in Shenzhen to farm out the job and clear 100% markup.We have full trust with our offshore PCB shops but it is worthwhile sending out RFQs to a few for their offers.So, the list (in order) for HDI (especially if you are not 'volume' driven yet):RichardShenZhen ChangSheng Circuits LimitedTell:0086-755-29668356Fax:0086-755-29668355Email: richard@cs-pcb.comWebsite:www.cs-pcb.com;AmyShenZhen ChangSheng Circuits LimitedTel: 0086-755-29668356 Fax: 0086-755-29668355Email Amy@cs-pcb.com Website:www.cs-pcb.comComments: Have used them in the past - the QC is excellent. Met them at past trade fairs in HK. Their offer for the SAME PCB fileset was about 50% for the HDI project @ ~$600 USD (landed with shipping to Canada).Daphne Tian (Ms.)Sales DepartmentMobile: +86-135-9019-1310KINGFORD PCB ELECTRONICS CO.,LIMITEDShenzhen Kingford Technology CO.,LTD.Tel: +86-755-23287851 ext:806Email: kfpcb12@kingfordpcb.comWebsite:www.kingfordpcb.comSkype: kfpcb12@kingfordpcb.comYour turnkey PCB & assembly partner in ChinaComments: Have used them many times in the past - the QC is always excellent. They often have a booth at the trade fairs in HK. They build PCBs for large companies including AMD. Their offer for the SAME PCB fileset was about 50% for the HDI project @ ~$600 USD (landed with shipping to Canada). They built our most recent 0.4mm pitch WLCSP bare PCB with full via-in-pad in our layout = Gowin FPGA.If you are into volume, shout back and will share more vendors who can support you. For us, we are constantly prototyping and the density of the devices just does not allow for hand building with the parts. Where possible, we use JLCPCB = dirt cheap and can build with our SMT line with < $ 250 (landed PCBs & stencil). This is a huge cost savings for us. Only issue is that JLCPCB CANNOT handle via-in-pad process. They are for the rather coarse PCB layouts only. Also their silk screening is quite low in quality. Then we use the above vendors or similar if with HDI. The larger shops will charge fixture fees, etc. but will be practical if your volumes are higher and the design is stable.

author: Harjit
author_rank: Regular Contributor
timestamp: October 02, 2021, 04:22:53 pm
content: Thank you for the detailed response. I'll check them out. This is only for prototyping/hobby project i.e. 5 to 10 pieces.Can you share details of the pad/footprint/stencil i.e. pad size, soldermask opening, trace width/spacing, via hole, via annular ring, solder paste stencil thickness and opening, etc. that worked for you?I did look at JLCPCB (https://jlcpcb.com//capabilities/Capabilities?_ga=2.210720981.1716972265.1618156606-862114027.1618156605) and here are the calculations for a four layer board - would love your feedback.WLCSP Pitch:0.4mmJLCPCB:* Min trace/space: 0.09/0.09 mm (3.5mil/3.5mil)* Min BGA Pad dimension: 0.25mm (9.8mil)* Min via diameter: 0.4mm* Min via hole: 0.2mm* Min via to track: 0.254mm* Soldermask opening/expansion: 0.05mm* Solder bridge min: 0.2mmGap to route n traces = n * 0.09 + (n + 1) * 0.09For 1 trace need a gap of 0.27mm.For 2 traces need a gap of 0.45mm.Per the JLCPCB minimum pad diameter = 0.25mm -> gap between pads = 0.4 - 0.27 = 0.15mm <-no traces can be broken out between pads.Diagonal gap between WLCSP pads = 0.4 * sqrt(2) - 0.25mm (pad size) = 0.57mmClearance between via diameter and WLCSP pads = (0.57 - 0.4) / 2 = 0.085mm <- maybe this is close enough to 0.09mm?Clearance between via hole and WLCPS pads = (0.57 - 0.2) / 2 = 0.185mm <- this misses the 0.254mm target. <-Cannot put a via between pads.Solder bridge = 0.4 - (0.25 + 0.05) = 0.1mm <-this misses the minimum solder bridgeThe lack of solder bridge worries me more.I've also done a bunch of research on what solder paste opening to use but it is unfortunately not conclusive.

author: mon2
author_rank: Frequent Contributor
timestamp: October 02, 2021, 07:31:54 pm
content: @Harjit, will ask our PCB designer on the specifics on the recently submitted job to JLCPCB and share the reply likely on Monday.I do know that JLCPCB rejected our original PCB fileset submission due to the 0.4mm WLCSP device layout (TI backlight boost regulator) and the BGA ball diameter with traces between the pads. The file set was then revised and they were fine with the revised file set. The job is in production now and we expect they will ship out next week or so (pending any of their never ending holiday schedules in China). The TI WLCSP device did NOT require the via-in-pad.Q: How many balls is your WLCSP device ?Respectively, are you requiring the via-in-pad in your PCB layout?The key reason being that after the fan out of each ball (ie. outer row / then next inner) - you will eventually be unable to sneak out the traces between the balls. For this reason, you will most likely need the via-in-pad process. At that stage, JLCPCB is out of the game. The via-in-pad process requires laser drilled vias inside the bga pad -> then a ring is made for conductivity to the next buried layer(s) -> then filled with resin -> then that same pad is topped up with another conductive pad. A royal pain for them I am sure and more $$$ we must dole out for the PCB.Another good shop but will most likely be also expensive isJETPCB.com-> they are in Taiwan and have produced amazing quality PCBs for us in small qty.We have used the following for our ICE40-WLCSP-16 PCBs with excellent results. In this case, we purchased in lots of 1000. The PCB did use via-in-pad process.NICOLE丨 TEAM LEAD OF SR. PCB SALES ENGINEERFAST TURN PCBT +86 (020) 2622 0250 | Email nicole.cai@fastturnpcbs.com | Website fastturnpcbs.comM +86 159 - 1574 - 3579 | Skype nicolecai2008 | What's app +86 159 - 1574 - 3579L Building 2401-2402, Dongling Plaza, Xintang Town, Zengcheng District, Guangzhou CHINAOn the solder mask under the WLCSP device - I do not believe this will be must of a concern. We build with these devices in-house and use the Loctite GC-10 no-clean solder paste. Highly recommended and has worked well for us on assorted PCBAs including the WLCSP designs. The stencils are sourced from JLCPCB. Suggest that you consider them as the first choice due to cost and consider alternates only if you run into serious issues. With the proper solder paste, the balls + paste literally fall into place like pillows / marshmallows melting. The need for the solder mask is not required. Honestly do not feel that many can support solder mask in this density but may be wrong here.

author: Harjit
author_rank: Regular Contributor
timestamp: October 02, 2021, 07:54:06 pm
content: I look forward to the information; thank you for chasing it down for me.It is a 33 pin WLCSP - info. attached. For my application, I can avoid the inner row breakouts but I think via-in-pad would be way better. I'll look up JETPCB, too.

author: mon2
author_rank: Frequent Contributor
timestamp: October 04, 2021, 11:47:12 am
content: @Harjit, sharing the comments from JLCPCB for our latest WLCSP based design submitted last week. They just shipped the finished boards this morning out of China.Hi Sir,Well got your order with many thanks~Sorry to bother you, but there is an issue that we want to confirm with you before proceeding.As shown below, 0.18MM BGA,0.09mm trace and 0.18mm spacing, they are not enough to proceed, please help to fix and keep 0.25mm BGA, 0.1mm spacing between trace and trace.Will ask our PCB designer for other specifics. If you can avoid via-in-pad, it will be beneficial in terms of PCB costs since you can remain with JLCPCB. Regardless, the stencil can be sourced through them. We use an Ekra X4 and purchase a framed stencil for our machinery. One of our engineers does the same for small protos without a frame and manually applies the solder paste + a Black & Decker toaster oven with success. At our site we use a 9 zone SMT oven for production.Avoid moisture on your devices as rapid heating of moisture exposed devices will turn to steam and cause silicon fractures / cracks = 'popcorn effect'. Seen this with seasoned SMT PCBA shops. The remedy here is to slow bake out the moisture using say 100 degrees C at 4+ hours. Then use on your PCB. If your WLCSP is supplied on a sealed tape - keep it sealed till it is time to apply onto your PCB.

author: voltsandjolts
author_rank: Unknown
timestamp: October 04, 2021, 12:33:56 pm
content: Quote from: Harjit on October 02, 2021, 04:22:53 pmFor prototype use, you could try using normal vias as 'via-in-pad'.With a small drill via, not tented on underside (to avoid trapped air) and perhaps some solder pre-fill, I doubt it'll wick much during reflow.Been meaning to try this but not had the opportunity yet.

author: mon2
author_rank: Frequent Contributor
timestamp: October 04, 2021, 04:03:57 pm
content: @Harjit, here is the feedback from our PCB designer on this topic:For our WLCSP, I had only one trace to route out between the pads. The two outer pads I changed to arounded rectangular shape that had the same surface area as the rest of the WLCSP pads. This willslightly alter the soldering shape of the ball but should not matter. This gave me enough room to routea 3.5mill trace with a 3.5 mil space on each side to the altered pads. This is within the published JLCPCBmanufacturing specs. Also there should be solder mask between all of the WLCSP pads. The pads are NSMD( non solder mask defined ) so the solder mask diameter is the same as the pad diameter. I also increased thesize of the remaining WLCSP pads to 10 mils from the original 9 mils so JLC would not have any issues.The minimum via I use is 20/10 - pad to hole size. Some folks complain about smaller sizes.Stencil apertures are 1:1 sized to the SMT pads except for the belly pads on some QFN or QFP packages.Many manufacturers will specify the aperture sizes for these packages. Most times the aperture is brokenup into a matrix of smaller apertures to limit the amount of solder paste applied.Hope this helps!My additional comments - allow for the SMT stencil shop (ie. JLCPCB) to define the aperture openings. They should know best. If you run into any issues, then proceed accordingly to tweak the stencil and try again. This formula has worked well for us to date and we are building with the referenced wlcsp density and devices. Again, if it can be avoided, skip the use of the via-in-pad process in your layout. It will be a lower cost if you can use JLCPCB. Otherwise, consider C&S and Kingford as noted above. Fastturnpcbs is also very good but there are savings to use the first 2 vendors as it is normal process for them using laser drilled vias.If you are really in a pinch, you can source stencils from a tier 1 shop in Shenzhen - Intel buys from them. We can share the full details on demand but is not necessary. Personally believe they do an excellent job but also their stencils will run you @ $ 150 USD for a 29" x 29" while the 'same' can be sourced for < $50 USD from JLCPCB, as an example.DO selectelectropolishingservice to remove burrs from the aperture openings in the SMD stencil due to the density of this layout.