Hi - I'm working on a really, really tight layout right now. I have a number of 0603 resistors very closely packed with a number of vias going to them. Would it be OK to place the vias directly in the center of one of a
0603's pads? This is for a prototype board, and will be hand assembled. Gut instinct says go for it, but my layout editor is yelling at me so I thought I should check just to be sure. Thanks,-Mike
unless you use a very, very small hole ($$$)
Cheers Terry
For hand soldering it might work okay, but it tends to wick the solder down the via, causing a dry joint or tomb stoning (the part is pulled up on one end during re flow soldering by the uneven surface tension).
google for via-in-pad.
It's sometimes used to reduce the inductance on bypass caps.
The usual problem is that the hole in the via sucks up some of the solder applied by the normal solder-paste through a stencil approach so there isn't enough left for a good solder joint. That shouldn't be a problem if you are hand soldering a proto board.
Make sure you have enough room to get the soldering iron in to solder the resistors.
-- The suespammers.org mail server is located in California. So are all my other mailboxes. Please do not send unsolicited bulk e-mail or unsolicited commercial e-mail to my suespammers.org address or any of my other addresses. These are my opinions, not necessarily my employer\'s. I hate spam.
Better yet, use same size hole on both pads, and centered.
unless its a big hole - reductio ad absurdum, it better be smaller than the pad.....
some contract manufacturers may refuse to make such a PCB.
Cheers Terry
Making the PCB? Why would they?
Of course, making the whole assembly is another matter.
-- Thanks, Fred.
Hello Mike,
I wouldn't do that. With one exception: When I need a really low impedance to other layers, for example in case of a connection area for chassis ground or a high amperage power supply cable (the garden hose size wires).
Consider smaller resistors. You can go much smaller than 0603 and nowdays smaller sizes are almost standard. But mind the dissipation, probably need to run ye olde HP calculator on every resistor that is low enough in ohms and across a few volts.
Regards, Joerg
dont laugh, i really have had contract mfgs piss and moan about IPCD275 and IPCSM782 - no comply, no build. And I meant populate the pcb, not fabricate it (although I have had a pcb mfg refuse to make single-sided PCBs with rivets, cant say as I blame them).
Cheers Terry
If you are hand soldering the you can get away with it. Otherwise use conductive via plug CB100 from Dupont.
Regards,
Boris Mohar
Got Knock? - see: Viatrack Printed Circuit Designs (among other things)
void _-void-_ in the obvious place
I think some fab manufacturers can solid-fill (plug) the via so the solder doesn't wick down the hole.
The problem with vias on pads that are soldered is that they develop circumferential fractures at the via/pad joint. Now if the via is solder filled, then the fracture may not bother you. If you hand solder them, it really makes them problamatic.
Al
On Sun, 09 Apr 2006 10:07:33 -0400, Boris Mohar Gave us:
All one needs to do is MASK over the via on the other side of the board.
On Sun, 09 Apr 2006 19:13:53 GMT, "Gary Pace" Gave us:
Solder mask is silk screened on wet. All he needs to do is make sure the mask covers any vias that he wants to keep wick free.
They only need to plug one side. It will not affect the via integrity.
"Filled vias" is what to google on. The hole-in-pad is doable but not all PC board vendors happily provide them and it is an additional cost.
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.