What is the default size of the via that you use and minimum value of via  - Page 1
Forum section: electronics / general

author: baremetal
author_rank: Newbie
timestamp: February 04, 2019, 10:39:02 pm
content: I know that this stuff really depends on the manufacturer capabilities but I was wondering what is default size of the via that you use and the minimum size that you feel comfortable using.

author: Warhawk
author_rank: Frequent Contributor
timestamp: February 05, 2019, 10:05:17 am
content: I use 10mil (0.25mm) traces as default together with 28mil (0.7mm) diameter and 12mil (0.3mm) drilling vias. I would somehow consider the 28/12mil via the industry standard. Every PCB shop can make it. I reduce dimensions with decrements of 2mils when I really need to. I always try to stay above the PCB house minimal requirements (not always possible due to tiny packages). Additionally, I keep 10- or (and) 5mil grid for components placement and routing. I typically avoid setting the grid resolution smaller than the minimum pitch of the smallest component on the board.For slightly higher-density boards, you can refer tohttp://www.ti.com/lit/ug/tidudo9/tidudo9.pdfchapter 4.3. There I go down to 6mils with a four-layer board and the single side components placement.I hope this helps.edit: To answer the second part of the question - I am generally uncomfortable with the drilling below 0.2mm. (8mil), annual ring below 6mil and trace below 6mil. This gives the size of 20/8mil for my smallest vias.Keep in mind that these are my personalized go-to settings when I do my projects and let them manufacture at shops like OSH park, Betalayout, SeedStudio etc.You can go for smaller sizes but you typically need to pay extra for smaller drilling etc.Also, this applies only to 1oz or 0.5oz copper plating. You may need to talk to the PCB house if you want a design with a thicker copper plating. Check design requirements from Betalayout. The webpage is helpful.

author: Rerouter
author_rank: Super Contributor
timestamp: February 05, 2019, 10:11:47 am
content: The smallest via size you can use that is within the manufacturing capability of almost all the cheap board suppliers is 0.3mm hole, 0.45mm pad,Now they may recommend 0.6mm pad, but every supplier I have seen that lists it, gives a hole positioning tolerance that would need to be exceeded to 200% to breakout the via pad, the pad could be smaller if not for the 8/8 copper rules.If the board isn't dense, I will generally just stick to 0.3/0.6 vias. means most of the time they get tented over by the silkscreen.

author: OwO
author_rank: Super Contributor
timestamp: February 05, 2019, 10:45:35 am
content: For 2 layer boards, 0.3mm/0.7mm via, 0.2mm/0.2mm traces/spacing is the lowest I'd go. I also avoid going too close to the fab house limits to ensure reliability.For 4 layer boards at JLCPCB 0.2mm/0.45mm is the smallest via supported, but I only use that for BGA routing and still stick to 0.3/0.7 whenever possible. Trace width/spacing I try to keep to >= 0.11mm for BGA routing, and >= 0.2mm elsewhere.

author: jeremy
author_rank: Super Contributor
timestamp: February 05, 2019, 11:45:22 am
content: I’ve never had any issues with 0.3/0.6 for vias and 0.15mm for traces. 0.1mm is reserved for extreme breakouts only, and widened out as soon as possible.

author: Kasper
author_rank: Frequent Contributor
timestamp: February 06, 2019, 04:13:48 pm
content: For my own stuff, built at cheap fab houses and hand assembled, I use 0.4mm vias with 0.8mm ring. I know that is bigger than needed but it reduces chance of problems, makes rework a little easier and leaves option to reduce them incase I ever really want more room for something on my board.For employers who want more expensive fab I go smaller.If you want to minimize via size, look into teardropping. When vias get small, drill accuracy becomes significant. If drill hits too far to side with track, it can disconnect track. Teardropping reduces the chance the track will be disconnected and allows you to use a slightly smaller ring.

author: xzswq21
author_rank: Frequent Contributor
timestamp: February 06, 2019, 07:37:46 pm
content: Quote from: baremetal on February 04, 2019, 10:39:02 pmyou can check the gerber file provided by some famous companies.usually I use 10/20 mils via (I mean hole size is 10 mils and the pad size is 20 mils). it's very clean. for clock signals I use 8/16mils vias and for some sensitive area I use 6.7mils laser via.the vias smaller than 12 mils (or 0.3mm hole size) could be tented by solder mask resin easily.

author: free_electron
author_rank: Super Contributor
timestamp: February 07, 2019, 01:48:47 am
content: laser 3 mils in 6 mil pad , stacked ELICfor your run of the mill board : 10 mil finished hole in 28mil pad ( they will drill with 12 mil ). every backshed shop can do that these days.