Few large via's or many small ones? - Page 1
Forum section: electronics / general

author: Simon
author_rank: Unknown
timestamp: June 05, 2018, 01:42:23 pm
content: If I am putting down via's for say the negative of a bypass cap than needs connecting to the ground plane underneath is lots of small ones or a few big ones best?

author: tszaboo
author_rank: Super Contributor
timestamp: June 05, 2018, 02:25:08 pm
content: related:https://www.eevblog.com/forum/projects/via-stitching-for-high-current-traces/"So but a bunch of via there. The smaller the better, I used 0.3mm vias. I made a test PCB just to test the optimal via size (for standard 35/70um 4 layer board ), because there was a fruitless discussion at that time at the company."

author: T3sl4co1l
author_rank: Super Contributor
timestamp: June 05, 2018, 07:33:51 pm
content: Few small ones. It's unlikely you actually need "many". That's more of a thermal thing.Some problems you can expect to encounter: not placing them optimally (following the current path), placing them too close to the pads (solderability issue), simply using more than is necessary, etc.Well, not so much problems as concerns really, but the point is, most layouts air on the side of superstition or ignorance rather than informed decision; the challenge is to know what physical properties you need from the board, and to design it accordingly.Tim

author: Simon
author_rank: Unknown
timestamp: June 05, 2018, 08:52:07 pm
content: Well in an ideal world i could have mahusive ground traces but this of course is not possible but I have 2 ground planes so can via straight down to them. Like you say via's in solder areas is a bad idea as it just sucks the paste away from the joint.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: June 06, 2018, 07:32:26 pm
content: Quote from: Simon on June 05, 2018, 08:52:07 pmI also meant near solder areas, because heatsinking. Makes hand rework a pain!Tim

author: Simon
author_rank: Unknown
timestamp: June 07, 2018, 11:11:31 am
content: It's a 4 layer board, reworking is going to be next to impossible anyway. The last time I tried to fit a missing part that was quite small to a 4 layer board it just ended up in the bin.

author: Eka
author_rank: Regular Contributor
timestamp: June 25, 2018, 05:43:51 am
content: A few small ones in the current path will work nicely. If you can't place them in ideal locations, then do what you can to keep the current path as short as possible. You shouldn't need any more via wall circumference than you'd need trace width to handle the expected peak current. More won't hurt unless it increases the length of the current path.

author: montemcguire
author_rank: Regular Contributor
timestamp: July 03, 2018, 05:20:04 am
content: Wall circumference is a good metric to keep in mind. Via hole size determines via circumference, and I usually use larger diameter vias for nodes like power or ground that would benefit from lower impedance. The height is determined by your stackup, so you can't control that. In my boards, vias go through the entire board, and there's a necessary keepaway distance, and disruption to all layers. I feel that this keepaway requirement favors one larger via than a few smaller ones. Inductance of the via will be reduced with a larger diameter, as it will using multiple parallel vias, but I think it's more efficient area-wise to use one larger via than a few smaller vias. Finally, I have only found a few instances when more than one large-ish via was good to use, and it was mostly related to needing to keep these vias arranged in a compact line.So, on the balance, I prefer one larger via over several smaller ones, as they seem more space efficient, and can have very low impedance if you scale them properly.

author: D3f1ant
author_rank: Frequent Contributor
timestamp: July 07, 2018, 09:24:43 pm
content: The Saturn PCB toolkit has a via spec calculator, you'll soon see which combination of a many small or one large works out better for your particular design. Since board makers done seem to charge per drill hole anymore, I tend to stick 0.3mm vias everywhere...the more the merrier.

author: IconicPCB
author_rank: Super Contributor
timestamp: July 10, 2018, 01:02:04 pm
content: Keep in mind via plating thickness is lower than outside layer plating thickness. Furthermore to the issue of hole wall activation many small vias may hide a defect in the plating of the walls when electrical testing is performed. Plating bath throwing power needs to be considered with high aspect ratio of PCB thickness to via hole diameter.