Looking for advice on in-pad via - Page 1
Forum section: electronics / projects

author: SpacedCowboy
author_rank: Frequent Contributor
timestamp: June 22, 2023, 04:29:06 am
content: So up until now I've always used the "dog-bone" via layout, and it's served me well, but it can rack-up the layer-count on the PCB for deeper BGAs. Looking at JCLPCB's capabilities pages, there's a section talking about VIA covering...QuoteThe BGA I'm thinking about has a 7-row-deep pad that I want to route out (together with 3 power planes: GND, +3v3, +1v8 - see below) and whereas the pitch is a friendly 0.8mm, it seems it'd be easier to do this if the via-in-pad option was chosen, I've just never done one before...So how does one go about setting this up (in Altium, if it matters) ? Do you create the normal pad, and then place the via inside it ? Or do you not bother with the pad, and just use the plated via since it's the same size anyway (if I'm using a 0.3mm land pad for the BGA, the via is 0.2+ 2*(0.05) = 0.3mm), which leave 0.5mm between the balls, and I can fit <space><trace><space><trace><space> into there with 0.09mm wide traces/space).That would mean 3 layers to route the 7-row-deep (3 rows on top, 2 rows on bottom, 2 rows on inner layer) which seems great - straightforward routing onto 6 layers total! so I'm assuming I'm missing something

author: Uky
author_rank: Regular Contributor
timestamp: June 22, 2023, 07:38:50 am
content: I have used JLPCB but not for complex/fine structure PCB's.Whenever I have designed boards with BGA's, there has been the headache regarding fanning-out.If there has been no room for thru-hole vias between the BGA pads, the use of micro-vias has beennecessary. If so, then:1. Crate the footprint the normal way with SMD-pads according to the datasheets suggestions.2. Create/Define/Use micro-vias size equal to or less (obviously) than the BGA pads where you define the hole to be plated AND copper filled. They can be placed right on the BGA Pads. Copper filled micro-vias is a must. Otherwise, there will be outgassing underneath the solder balls that pops solder once the board is in the reflow oven. The use of micro-vias requires the layer "TOP" to "INNER1" to be very thin. In the past, this layer was specified as RCC (Resin-Copper-Clad) and in my cases, about 0.1mm but manufacturing may have made some progress since then.3. Once the connection has hit the first inner layer, you are at liberty do proceed with the stackup according to the chosen board vendors recommendation. Normally, a symmetrical build is recommended. Otherwise, there will be a risk of the PCB becoming warped/twisted during reflow soldering process.You also will need to check the current carrying capabilities of the micro-vias just in case..."My 5 cents"

author: Solder_Junkie
author_rank: Frequent Contributor
timestamp: June 22, 2023, 08:07:32 am
content: I’m not very experienced at commercial PCB production, only had a few made. But one of my basic designs was quite cramped and I considered using vias through pads, but if I remember correctly either the design software rule check, or the JLC PCB design check, threw up an error with that approach.My gut feeling is that vias in-pad are best avoided, but there again my boards aren’t that complicated.SJ

author: Marsupilami
author_rank: Frequent Contributor
timestamp: June 23, 2023, 02:20:22 am
content: Via in pad should be a no-brainer imho, considering it's free at JLCPCB. I'm sure there are subtleties, like how much the overplating sags under the BGA balls vs solder volume etc., but still I don't think you can go wrong with it. It's an extra free routing layer for fanout.Another good use case for it is when short paths are required for example in thermal pads under ICs or ground terminals of RF or high speed connectors, but also don't want solder to be sucked out through an array of vias.