EEVblog Electronics Community Forum
Electronics => Projects, Designs, and Technical Stuff => Topic started by: firstcolle on September 25, 2018, 07:28:29 pm
-
I'm wondering if it's a good idea to put vias under smd 0805 pads,like the picture attached
-
Depends. Are you hand assembling? Go ahead. Are you mass producing? via-in-pad can cause serious assembly issues if you don't take precautions like filling the vias. Solder can wick down via during reflow starving the joint or causing tombstoning. It depends on the via diameter and the type of solder (leaded solder is worse). If possible, try to move the via out of the pad and possibly tent with solder mask. If not, consider if you can use filled vias. The normal process is to make the via, fill with epoxy, then plate over the top so that you get a smooth pad surface. That does increase your PCB cost due to the added steps.
-
I have done this plenty of times with little to no problems, as ejeffrey said, if you are hand assembling then go ahead, if you are making a product that will be mass produced then try your best not to, to avoid QC problems.
-
If you can avoid it, don't put a via in a pad under any circumstances. It makes the component unstable and can trap gases.
-
If you can't avoid what you have done, at least add thermals to the GND via, in the other layer(s) where it connects to the GND plane. This way:
1) Thermal conductance of that GND via is reduced, which makes soldering easier
2) Imbalance between the thermal conductances of the two pads is decreased (i.e., they are more close to each other in the amount of heat flow required), so that the risk of tombstoning is decreased in production.
Use as small vias as possible. 0.4mm is really pushing it. With 0.3mm, you have some chances - solder wicking effect is reduced (and the thermal resistance is higher). With 0.25mm, I'm typically having success in via-in-pad, but still, I only do it in the large pads of power devices.
If you look for an actual hard design rule, then the answer is simple: no, you can't do it - or only if you use 0.1mm laser micro vias - they have sufficiently low thermal conductance and no solder wicking occurring. If you can't afford HDI fab, 0.2mm drill is very likely to succeed (given minimal via diameter on the other layers, and sufficient thermal reliefs connecting to planes.)
Also note while others have gave you "go ahead" for hand assembly, these kind of direct vias to a large ground fill can be pain-in-the-ass to hand-solder as well! The only difference is, you can't avoid doing "quality control" while you solder, and just end up using more time and curse words, but it won't be a showstopper like in mass production.
-
Depends on how you solder it. With paste, no, don't put vias on pads as chances are good it will suck down your paste leaving you with a partial or nonexistent joint. You'll solder the board, then inspect it and wonder why this one is dry??? Apply more paste, hot air, solder it, inspect and huh, no solder! Then repeat until you've filled the via. Scratch your head until you eventually realize that pad has a via. (Been there done that, not worth the hassle.) An exception is if you have it plugged, because you really really need a via in an inconvenient spot like under a BGA ball or QFN pad. Or if you drag solder in which case the via volume won't make any difference - there will be piles of solder to go around.
-
Why.... just why? :palm:
When you'll put your hands on the board after one year and try to do some troubleshooting, you will have your answer. :-/O
-
Here is another way of arranging the vias that prevents the holes from wicking solder. For reference, the footprint is 0805 Min and the via holes are 0.2 mm with 0.15 mm annular ring. Make sure that the solder mask is completely covering the holes.
-
An other way to do it. A track can be laid out between the vias.
-
You should avoid via in pad if possible, because that will decrease the yield. Via in pad for QFN is generally fine, because you don't need 100% coverage for power dissipation to be perfect. If you do it for QFN, stick to 0.3mm vias. For 0805? Just why? Just use smaller component, have the via next to the part. Tent the via.
-
As already mentioned, for hand assembly it will usually be perfectly fine.
For automated assembly, it will require the vias to be filled. That's a process that's just typically referred to as "'via in pad" by PCB manufacturers. This is usually an expensive option.
It's interesting, or even sometimes mandatory, for very dense designs with fine-pitch BGAs or such. But for 0805 components? If you're doing it just because you find it looks nice and tidy, I'd suggest not doing it and sticking to using vias outside of pads. If you do this though, you'll need a good reason.
-
An other way to do it. A track can be laid out between the vias.
Be very mindful of your tolerance stackups on trace width, solder mask expansion and solder mask alignment before doing this. A 4 mil expansion and 4 mil alignment tolerance and a trace that's 1 mil oversized can make for that trace that was a whopping 9 mil away before, is now exposed and ready to cause a short to the pad.