0805
ng an
You can put the via right on the edge of the pad, but make sure the hole is beyond the pad. Tent all the vias, which means they are dropped out of the solder mask artwork. Then there are no soldering issues and no long trace issues. If your layout package doesn't support tenting vias, it can be done manually by deleting that d code and flashes from the gerber file for the solder mask. Then check it with software like Viewmate before ordering the board.
Yes, but you cant usefully soldermask a via which goes through an SMD pad.
Lots of people have given you the correct advice here. However if you want to go googling, the correct term is "via in pad" which for some reason no one has said.
Colin
On Mon, 6 Jun 2016 09:14:08 +1000, Adrian Jansen Gave us:
No. You mask a pad that goes NEAR an SMD pad. If you were to mask one that goes 'through' an SMD pad, you would be masking off some of a pad meant to attach a part.
I am sure that would make for an interesting stencil as well.
Generally true, except for large thermal pads where multiple vias are required, where a soldermask grid isolating the vias and dividing a large pad into multiple smaller pads can be a cost effective way to avoid solder wicking down vias and also help reduce voiding by providing shorter gas vent paths.
This technique would likely work well even with toaster oven assembly.
Glen
My software (sprint layout) doesn't have a via, so I'm playing around with a square pad and through hole.
Right now I have it as a 30 mil square and 15 mil hole but what's a typical size and how small can I get away with without a problem when being fabricated?
On Tue, 7 Jun 2016 13:08:12 -0700 (PDT), mkr5000 Gave us:
You'd be better off using Linux and one of their free EDA packages.
15 mil is a bit conservative. I often see 13 mil holes minimum for low cost board fab houses. The annular ring is usually measured by the width (think radius rather than diameter). 15 mil hole and 30 mil pad gives 7.5 mil pad which is better than the common 7 mil minimum at the low cost board fab houses.
-- Rick C
I generally stay away from vias in pads at all costs but here are some tips if you feel you must:
Superfast stuff like my fave BFP640 really needs via-in-pad, preferably two or three of them. It's a 40-GHz transistor, and an extra nanohenry in the emitter lead makes a big difference. (1 nH is 63 ohms at 10 GHz.)
(1 pF and 1 nH make a parallel resonance at 5 GHz. Also a cause of endless fun in debugging oscillations.)
Cheers
Phil Hobbs
-- Dr Philip C D Hobbs Principal Consultant ElectroOptical Innovations LLC Optics, Electro-optics, Photonics, Analog Electronics 160 North State Road #203 Briarcliff Manor NY 10510 hobbs at electrooptical dot net http://electrooptical.net
I touch various nodes with a pencil or the tip of a tiny screwdriver. If anything changes, something is probably oscillating.
I recently did a diff pair with a couple of BFS17s, and it didn't oscillate! I might try something faster.
-- John Larkin Highland Technology, Inc lunatic fringe electronics
*gasp* ;)
BFP640s with those nice little Murata BLM18BB005 beads in the base lead are pretty stable up to about 5 or 6 mA I_C.
Cheers
Phil Hobbs
-- Dr Philip C D Hobbs Principal Consultant ElectroOptical Innovations LLC Optics, Electro-optics, Photonics, Analog Electronics 160 North State Road #203 Briarcliff Manor NY 10510 hobbs at electrooptical dot net http://electrooptical.net
-- Or, perhaps, was OK before you threw that pencil or tiny screwdriver monkey wrench into the works? I'm constantly amazed at the effort you expend in order to glorify yourself and, after all's been said and done, haven't figured out why why your foot still hasn't left your mouth. John Fields
On Wed, 8 Jun 2016 11:40:32 -0400, Phil Hobbs Gave us:
Good point. How much different do they behave when solder filled or left empty?
Not a lot, I expect, though I haven't tried measuring it. The inductive reactance is way bigger than the resistance of even an empty via.
Cheers
Phil Hobbs
-- Dr Philip C D Hobbs Principal Consultant ElectroOptical Innovations LLC Optics, Electro-optics, Photonics, Analog Electronics 160 North State Road #203 Briarcliff Manor NY 10510 hobbs at electrooptical dot net http://electrooptical.net
When inductance to ground matters, we'll usually dump a pour around the lead and drive multiple vias to the layer 2 ground plane, or use multiple caps. My production people won't give me pizza if I put vias in pads.
-- John Larkin Highland Technology, Inc picosecond timing precision measurement jlarkin att highlandtechnology dott com http://www.highlandtechnology.com
Sometime you should try filled vias. Your production people shouldn't have any trouble with them. They cost but you don't do millions a year. You'd probably not notice the cost.
I haven't needed it so far. We have put some vias in pads, mostly for heat sinking powerpad parts, but not so many/so big that we get solder stealing. Copper fill might be nice, epoxy not so much. If the heat transfer path is layer 1 to 2, it's a pretty short hop and fill might not help much. Side-to-side would benefit more.
I generally avoid exotica unless there's a big payoff.
-- John Larkin Highland Technology, Inc picosecond timing precision measurement jlarkin att highlandtechnology dott com http://www.highlandtechnology.com
Solder fill works.
I'm suggesting that you try it before you need it. It should be pretty easy to do a test site on one of your boards. Get the production guys used to it so they don't revoke your annual bonus. We do the same with ours (0201 parts, .5mm BGAs, etc.).
OK, I guess I might ask at least. What I really want to do next is some fast circuits on kapton flex.
-- John Larkin Highland Technology, Inc picosecond timing precision measurement jlarkin att highlandtechnology dott com http://www.highlandtechnology.com
ElectronDepot website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.