Why are uVias from top layer not standard with the cheap manufacturers? - Page 1
Forum section: electronics / general

author: jusaca
author_rank: Unknown
timestamp: March 31, 2022, 02:13:45 pm
content: Having uVias between inner layers requires the manufacturer to pull the boards from the etching and pressing process to laser drill the vias (and even close them, if additional vias should be stacked on top). This is obviously some decent amount of extra work, so I totally get why this is only available in special HDI board lines.But having uVias from top layer to one layer below seems to me to be a pretty cheap addition to only PTH. The manfacturer could place the finished panal in a standard laser system, drill the uVias to the layer below and it's done. That seems to me to be even cheaper, if it reduces the amount of physically drilled holes.The big advantage would be, that even a cheap standard process would allow via in pad on the the pcb side with the smd components and you could easily switch layers below the package, without having to disturb the GND layer.I get that a lot of boards don't really need uVias, but because adding them to the top layer does not add a lot of cost (at least in my head, maybe that's a completely wrong assumption) I can't see why manufacturers like JLCPCB don't offer that possibility.So, what is the big catch? Why would uVias on the outer layer be hard / expensive to do?

author: mikeselectricstuff
author_rank: Super Contributor
timestamp: March 31, 2022, 04:02:29 pm
content: Depends on their process, but AIUI boards tend to be built from the inside out, so L2-L3 is easier than L1 to L2

author: langwadt
author_rank: Super Contributor
timestamp: March 31, 2022, 04:33:10 pm
content: Quote from: mikeselectricstuff on March 31, 2022, 04:02:29 pmatleast for impedance controlled, JLC shows the stackup as L2-L3 on a core and the L1, L4 with prepegbut still, I imagine going from L2-L3 would require drilling and plating the core before adding the outer layers, where as going from L1 to L2 would only require making a blind hole from L1 to L2 before the normal plating of out layers and regular vias

author: jusaca
author_rank: Unknown
timestamp: April 01, 2022, 07:02:36 am
content: Exactly, burried Vias seem to be quite some more extra work, drilling and plating before pressing the outer prepreg on.But with uVia from L1 to L2 it seems to me to be really fast.With laser drilling the uVias you can simply "shoot" at the outer layer (you only need to etch a tiny hole in the copper in the middle of your via) and the prepreg vaporizes. Depending on the laser wavelength you use the laser automagically stops at the next copper layer, leaving you with a perfect via between L1 and L2. And because this via is soooo tiny, it is absolutly no problem to place it inside of pads.

author: Doctorandus_P
author_rank: Super Contributor
timestamp: April 09, 2022, 10:37:04 am
content: As long as you're talking "cheap manufacturers", then you are looking at a standardized and simple process, which means drilled holes.There probably is not even a laser in the same factory as where those PCB's are manufactured.

author: jusaca
author_rank: Unknown
timestamp: April 11, 2022, 10:20:19 am
content: Well, yeah, I get that. The question iswhy.A laser system is cheaper than the mechanical drill bits, in the long run. Plus the addtional benefit of beeing able to advertise uVias (even if only on the top layer). So I would assume all the el cheapo manufactureres to run off and by laser systems.Because that seems not to be happening my reasoning is probably wrong, but I can't see where it is wrong... Are laser drill systems so much more expansive than I imagine? Is the aligning of them so hard?

author: mikeselectricstuff
author_rank: Super Contributor
timestamp: April 11, 2022, 11:08:11 am
content: Quote from: jusaca on April 11, 2022, 10:20:19 amI'd be interested to know more about this - my guess is lasers can only do tiny holes ( or are only economic for this in terms of cycle time). I would be surprised if a laser is cheaper than a mechanical drill.Then there is the produciton throughput - A mechanical drill can drill through multiple panels in one pass, and PCB drills often have multiple heads, so a single cycle can drill a lot of holes.

author: jusaca
author_rank: Unknown
timestamp: April 11, 2022, 11:21:26 am
content: Yes, you are right, you can't replace the mechanical drill. The laser is only used to drill through one layer (the typical laser only drills through resin and will not damage the copper below) and typically creates via diameters between 75um and 150um.But you can reduce the number of necessary mechanical drill holes, when most of the connections between SMD components can happen on Top + the layer below.Quote from: mikeselectricstuff on April 11, 2022, 11:08:11 amTrue, you can only drill panel by panel with a laser, but all holes basically are drilled in one flash. You don't have to move the drill bit over the panel, you just change the angle of the mirror to direct the laser. It really is just one flash of a fraction of a second and you have all your laser vias drilled.According to the slide in the attachment the laser system drills >150 vias/s. And that was 8 years ago.

author: Marco
author_rank: Super Contributor
timestamp: April 11, 2022, 12:42:09 pm
content: Uncertain return on investment probably. A lot of the drilling machines are presumably refurb, the laser would might have to be brand new. If all the customers who need it just stick with the higher cost/volume manufacturers and your own customers are used to doing without and go for the cheaper option, you're screwed.

author: Psi
author_rank: Super Contributor
timestamp: April 11, 2022, 12:54:29 pm
content: You would have to get quotes from professional non-hobby pcb fabs in quantities above 10,000 in order to compare how much extra it actually costs to have laser via's in various configurations.But even then,. As soon the fab hear "laser via" they know they can charge you more. Even if there are some configurations where adding limited laser via's is easy/cheap for them, they probably don't want to tell you that.You would likely have to negotiate that info out of them. Lots of back and forward communications trying to get them to lower cost and them making cost concessions only if you limit laser via's to specific layers etc..

author: Feynman
author_rank: Regular Contributor
timestamp: April 17, 2022, 07:20:44 am
content: Pooling manufacturers want to have as little differences between the designs as possible in order to have maximum panel efficiency. Keep in mind that having micro-vias will most likely require a special stack-up: Laser drilled micro-vias shouldn't be any bigger than 0.15mm. To get good plating the aspect ratio should be around 1:1 so the prepreg between outer and first inner layer can only be 0.15mm thick (many fabs prefer even thinner prepregs). That is certainly not a "standard" 4 or 6 layer stack-up anymore. Plus plating micro-vias is a different process than plating thru-vias (may depend on the fab).Speaking of plating micro-vias: Return on invest on machines is one thing. Process knowledge is another.And it's not like you can get rid of the mechanical drilling process. You still need mechanical drilling for thru-holes.But laser-drilled micro-vias are certainly no black magic either. We regularly order PCBs with laser-drilled micro-vias from outer to first inner layer and they don't add any significant cost with our lot sizes (low 4 digit figures). But that is just gut feeling. We never actually compared the price of two versions of an identical design - one version with, one without micro-vias (kind of pointless). The net cost is very likely lower with micro-vias, because of reduced board size and/or reduced layer count.If demand increases more fabs will offer micro-vias for sure. But demand isn't in the "sweet spot" for cheap pooling manufacturers just yet, I guess.Maybe we just have to wait until used laser drill equipment trickles down from high end to low end manufacturers.

author: langwadt
author_rank: Super Contributor
timestamp: April 17, 2022, 07:58:31 pm
content: Quote from: Feynman on April 17, 2022, 07:20:44 amJLCs impedance controlled JLC2313 4/6 layer stackup is 0.1mm outer layers

author: T3sl4co1l
author_rank: Super Contributor
timestamp: April 17, 2022, 08:14:34 pm
content: It might sound obvious enough from an idea perspective, but that's just one out of many reasons for or against doing it.For example, you've perceived an opportunity; but how often would you actually make use of it personally? Is this just one board you're working on that would benefit? How many others would, then? What about other customers? Finally, how often will it show up in the total production flow at the fab itself, and is that enough to justify adding the process step?But you don't really know. Manufacturers even, don't really know -- there's a bit of a chicken-egg problem, no one orders it because no one offers it. At least at such a price point. Laziness being the default, it would seem an unlikely step to take -- that's a lot of capital cost, for something extremely price sensitive already, and of dubious value.If an illustrative example can be made by moderately priced fabs for example, maybe the cheaper ones would consider adopting the process -- they aren't going to do anything that isn't well proven and cost effective -- but here again, very few are doing it, so it seems to be unprofitable. Maybe again the problem is it's a nonstandard option, so, a cost adder, its popularity artificially suppressed from the actual equilibrium price, if only it were to became the norm -- but so it goes.Tim

author: jusaca
author_rank: Unknown
timestamp: April 19, 2022, 09:38:43 am
content: Well thats true, using uVias limits you in what stackups you can use. That might really be part of the reason, probably combined with all the uncertainties T3sl4co1l mentioned.Would certainly be cool to be able to order uVia-Boards at JLCPCB prices in the future