HDI Tips and Tricks - Page 1
Forum section: electronics / general

author: anguyenle
author_rank: Newbie
timestamp: August 28, 2019, 09:40:03 pm
content: Hi Everyone!New to this forum, but also surprised by the lack of quality suggestions on how to design HDI boards for cheaper. For example, there are people who will say things like "you need via-in-pad for 0.4mm pitch BGA" when I know for a fact that I have made designs work without doing that, and have seen literature containing tips that will help you avoid via in pad. If anyone is willing to share some of their HDI tricks, I'd be extremely grateful, some of the ones I've found which have worked are:- BGA oval pads: There's a nice study herehttps://www.keysight.com/upload/cmc_upload/All/CUSTOMER_5DX_UGM_Oval_Pads_030105.pdfwhich demonstrates that using oval pads can be more reliable and (not demonstrated, but obvious) can help with fanout. In my own designs, I've used oval pads (not rotated as in the study, it didn't help in my own design) to give myself a little bit of extra space to fit within the 3/3 or even 5/5 tracing specs with designs that have worked totally fine. There is very little literature on the reliability of these pad styles other than a couple of papers saying that they are sometimes more reliable, but at least you can bring a $5000 HDI design down to a $2500 one. For prototyping, these kinds of tricks are invaluable.- Ultra thin traces: I've found that it's often cheaper to go with a manufacturer that can print sub 3 mil traces if it saves you from using a ton of buried/hidden vias in your design. Obviously, drilling aspect ratios will vary from manufacturer to manufacturer so sometimes this isn't the case, but whenever pcbs with 8 layers (or more) come into play, I've found much longer lead times and way higher costs associated a lot of different drilling schemes that aren't nearly as bad with thinner traces. This leads into my next point- Staggered vias: This one isn't so new anymore, if you google it you'll find out exactly what I mean really fast. It's both more reliable than stacked vias and cheaper, yet when you look at some recommended fanout patterns, some manufacturers recommend stacked vias exclusively despite the design not requiring them and IPC design standards explicitly not recommending them. This makes the fanout patterns from some manufacturers useless because the second you call your fab house, sometimes they'll shrug their shoulders and say, well if you stagger them, then you'll have something a little more reliable.Also, I'm quite sure I'm full of crap so if you can find a study saying you shouldn't use some of these tricks, that would be much appreciated!

author: Dubbie
author_rank: Unknown
timestamp: August 28, 2019, 09:55:09 pm
content: I would be really interested to hear how you do 0.4mm pitch without via in pad?What manufacturer do you use?A lot of really nice small parts only come in 0.4mm pitch now.

author: anguyenle
author_rank: Newbie
timestamp: August 29, 2019, 06:49:37 am
content: Quote from: Dubbie on August 28, 2019, 09:55:09 pmImagine what happens when things move the 0.3mm. It's quite hobbyist unfriendly to say the least. You have to respond with a trick that you've learned that isn't super popular since I shared that oval bga pad thing.Since the "annular ring" requirement can go as low as 2 mils, you can use the dogbone fanout pattern contrary to popular belief, just use the minimum size vias with minimum size annular ring. Unfortunately, I'm not at my work computer and thus cannot access Altium to prove that this does not violate 3 mil spacing constraints. Perhaps tomorrow. Some people will say via in pad is more effective, but I can't see why for a smaller device. You'll pay more, have slightly worse signal integrity, have a lead time that is roughly doubled, and have so much extra communication with your fab houses when you're comparing between them because the DRM are all slightly different.As for interesting manufacturers, Advanced Circuits can laser drill a 3mil hole, Sierra Circuits can drill 2 mil holes AND completely plate it over (but I've never done this) to end up with something resembling a via-in-pad without the associated filling steps.

author: Dubbie
author_rank: Unknown
timestamp: August 29, 2019, 07:23:56 am
content: Yeah last time I started talking to Chinese fab houses about via in pad, it got so confused that I gave up and switched to a different footprint part. Maybe l’ll have a go at dog bone fanout. I try to avoid blind vias usually, so for small parts, it might be doable if I get lucky with pinouts.

author: Brutte
author_rank: Frequent Contributor
timestamp: August 29, 2019, 08:25:09 am
content: Quote from: anguyenle on August 29, 2019, 06:49:37 amVia in pad does not have filling step and no additional data has to be provided. Soldermask comes in one of the input files. And via-in-pad in HDI is typically made by laser (50x cheaper and faster than drilling with drill but only goes through thin prepreg).Most likely you are confusing via-in-pad with plugged via or capped via. These are different animals.BTW, I would like to see your 0.4mm bga without via-in-pad. I just hope this is not a 2x2 bga.

author: anguyenle
author_rank: Newbie
timestamp: August 29, 2019, 10:38:51 pm
content: Quote from: Brutte on August 29, 2019, 08:25:09 amI sense some animosity, but maybe I'm too sensitive. Feel free to share a tip if you have any, I'm here to learn and I encourage you to have the same attitude.https://www.protoexpress.com/via-in-pad-features.jsphttps://www.mclpcb.com/vias-bga-pads/https://www.7pcb.com/blog/difference-between-via-tenting-and-via-in-pad.phpHere's two links using the exact same language to describe via-in-pad. When I say via in pad, I'm referring to vias that are filled with epoxy (conductive or nonconductive, depending on your requirements), then flattened and capped with your conductive material to ensure planarity. Unfortunately, a lot of people will call this a via in pad and I've never been corrected with such conviction that a capped-via-with-an-epoxy-fill is not a via in pad by my fab houses so please excuse my mistake. This is design has been fabbed, and working but maybe its reliability isn't great.This of course isn't the end all and be all, but this is an FPGA with 64 user accessible IO, and there is no via-in-pad here. Advanced circuits said that this is the limit of their capabilities, but I cut my lead time from 20 days with a VIP design to a 10 days, and cut the cost in half. Further optimization is possible of course, but this design needed to get pushed out FAST so it may not be up to a perfectionist's standards. However, this is a dogboned 0.4mm pitch design. It's 11x11, and I bet that if you asked this question to yourself, you would have required yourself to use via in pad because of the dearth of opinions saying that its necessary or more efficient. There are only 4 maximum rows and columns you really need to fan out. Ovals made the outermost ones pass DFM, and I made the board thickness really thin so that you could still drill layers 1-4 mechanically because the vias stacking was super duper expensive. I didn't try to stagger the vias because I just wanted to test this out and it worked out fine. I wish I'd done that to get a cost comparision. I realize now in my screenshot that i didn't include a scale bar, but the pin pitch is 0.4mm. If you try the things I suggested earlier, you too can make this work.Also I didn't know laser drilled vias were cheaper. I thought that the sequential lamination process makes mechanical drilling cheaper if you can make your board super thin. I'd love to discuss my design more, but I'd love it even more if somebody could provide some sweet tips for this kind of stuff.

author: Dubbie
author_rank: Unknown
timestamp: August 30, 2019, 02:20:27 am
content: Have you got soldermask on that?

author: Brutte
author_rank: Frequent Contributor
timestamp: August 30, 2019, 06:07:30 pm
content: Your 0.4mm BGA epoxy filled via-in-pad seems like a laborous process. I did hear about the possibility of filling vias with epoxy but what you show is really crazy (and expensive I suppose). What is the drill size in your design?I was talking about laser drilling via-in-pad asdescribed here in WE.

author: nctnico
author_rank: Super Contributor
timestamp: August 30, 2019, 08:19:57 pm
content: The idea of having oval BGA pads is intriguing. I have an HDI design where I had to shave some BGA pads to make room for traces (already 0.9mm/0.9mm). Using oval pads could bring back a larger soldering area.

author: KE5FX
author_rank: Super Contributor
timestamp: August 30, 2019, 09:00:06 pm
content: Maybe I'm missing something from the .PDF, but it seems like they are using oval pads to make opens show up more readily during X-ray inspection, not as a way to hack around trace/space restrictions at the fab house...In that 0.4 mm design, I wouldn't be worried about board fabrication as much as soldering. Those stencil openings are going to need to be unusually small, aren't they?

author: anguyenle
author_rank: Newbie
timestamp: August 31, 2019, 12:47:57 am
content: Quote from: KE5FX on August 30, 2019, 09:00:06 pmThat is one point of it, but I went for it because it's just a way to make it work and I found some support literature showing that it won't just fail. The paper this study quotes also discusses the better strength that oval pads affords. The stencil openings being small is no big deal though, remember that this part is cut with a laser and that diffraction limited spot sizes are on the scale of microns while the pad itself is roughly on the scale of 100-200 microns. Furthermore from the picture, I bet you can't really tell that the outer BGA pads are ovals. I sure can't, but it makes it pass DRM and even if it didn't, just find a manufacturer that is ok with 2.75/3. You might have to have a half ounce of copper on the outside, but it sure beats paying so much for filled vias.Quote from: Brutte on August 30, 2019, 06:07:30 pmIt was pretty expensive, but I didn't really make the pads that oval. I got a quote from pcbway and if I made them more oval, I bet I could work this design into a 3/3 width/spacing. My stacked via design was roughly 1.8K for 10. I'd estimate it would be 1.2-1.5K for the ovals but at a shorter lead time. Also, if the pad isn't flat, you could end up with issues from outgassing/wetting leading to voiding during reflow. They're mentioned here on slide 35-39, but perhaps Wurth has a specific process for mitigating these issues since they're advertising that type of via. Maybe they're using the smaller solder paste composed of smaller balls or overplating it completely?https://www.smta.org/chapters/files/Voids_in_Solder_Joints___Intermountain_SMTA_Chapter_March_2018.pdfBottom line is I'm pretty unnerved by that style of via--more than I am about the oval pads, but the oval pads technique isn't broadly published so it may also be subject to less scrutiny. Completely plating over blind vias is obviously a viable strategy if and only if your boardhouse can do it cheaply and reliably. Otherwise, I see no real advantages over doing this using dogbone fanout.