Does it matter if SMT pads are REALLY close to each other?

Thread Starter

ebeowulf17

Joined Aug 12, 2014
3,024
Hey everybody, I'm working on redesigning an existing board layout to accommodate different connectors, and it's made the layout pretty cozy. I've got two 1206 resistors whose pads are basically touching, and I'm wondering if that's a problem.

They're part of the same node, and connected by traces anyway, so I'm not worried about electrical connections. All I'm wondering is if having the pads essentially merge into one has any risks in terms of manufacturing processes. Will the solder paste on the two pads make a different shape? Does molten solder have a surface tension that will make it pull towards the center of the combined mega-pad (and away from the components?) Are the connections more likely to fail when their pads don't have the usual well-defined borders with soldermask in between?

This will be mass produced, with pick and place machines, reflow ovens, etc. so I'm not worried about hand-soldering (although repair/rework may be more difficult with tight spacings and thermal coupling.)
upload_2019-2-22_8-1-21.png
 

Attachments

MrChips

Joined Oct 2, 2009
19,910
I don't see an issue If the two pads are connected. If I were hand soldering, sometimes I would allow the pads to overlap or share a common pad if that provides some benefit such as saving space.

I don't know if that will flag an error in DRC or cause problems with pick and place machines. I would be inclined to make them touch so that there is zero gap between the two, if it passes DRC.
 

kubeek

Joined Sep 20, 2005
5,654
If you are going for automatic reflow then this could create issues. It might not be possible to create that very thin bridge on the stencil which could lead to too much paste, and you could have problems with the resistors shifting or tombstoning. It could possibly be cured anyway with tweaking the soldering profile, but I would try to avoid it in the first place.
 
Last edited:

Thread Starter

ebeowulf17

Joined Aug 12, 2014
3,024
Thanks to all of you for your comments. It sounds like there are a number of legitimate reasons to avoid this, so I'll do some rearranging and put a little space between them. It won't be much, but I'll make there's enough room for a thin web of solder mask to keep them separate.

One more question on this design while I've got your attention - do vias which are too close to pads bring similar risks? Should I be worried about my tight vias on R2, OPTO1, Q1? My gut feeling is that thermal effects will be minimal, so the only real risk would be losing solder to the inside of the via hole. That could be mitigated by requesting tented vias, right?

Thanks for all the help. Cheers!
 

MrChips

Joined Oct 2, 2009
19,910
Again, my response is similar to the one before. I put vias right into the middle of an SMD pad with no problems.
It has never been rejected by the PCB houses. Try it and see if it works.
 

ian field

Joined Oct 27, 2012
6,539
Thanks to all of you for your comments. It sounds like there are a number of legitimate reasons to avoid this, so I'll do some rearranging and put a little space between them. It won't be much, but I'll make there's enough room for a thin web of solder mask to keep them separate.

One more question on this design while I've got your attention - do vias which are too close to pads bring similar risks? Should I be worried about my tight vias on R2, OPTO1, Q1? My gut feeling is that thermal effects will be minimal, so the only real risk would be losing solder to the inside of the via hole. That could be mitigated by requesting tented vias, right?

Thanks for all the help. Cheers!
There are pin/pad spacing regs for mains isolation - probably worth giving them a read.
 

Wolframore

Joined Jan 21, 2019
1,514
The only issue I can think of at this point is that the via could suck all the solder into it's hole. I have seen via's on pads but usually they are filled with epoxy (expensive).... If you have the space for it always leave at least the trace width away... again just good practice.
 

Thread Starter

ebeowulf17

Joined Aug 12, 2014
3,024
There are pin/pad spacing regs for mains isolation - probably worth giving them a read.
I think I found good info on isolating the mains side from the low-voltage DC side at the following link, and I believe I've got that covered.
https://www.smps.us/pcbtracespacing.html

I'm less confident about how much space I need between all the various pads and pins on the high voltage side. I suppose I should do some more research on that and make sure I'm not creating some sort of arcing potential - it wouldn't be a shock hazard for anyone on that side of the board, but could maybe still be a fire hazard or at least impact reliability. As usual, more homework to be done...

If any of you have especially good resources on this issue, specifically for mains voltage up to 240 or 250VAC, I'm all ears!
 

WBahn

Joined Mar 31, 2012
25,060
Hey everybody, I'm working on redesigning an existing board layout to accommodate different connectors, and it's made the layout pretty cozy. I've got two 1206 resistors whose pads are basically touching, and I'm wondering if that's a problem.

They're part of the same node, and connected by traces anyway, so I'm not worried about electrical connections. All I'm wondering is if having the pads essentially merge into one has any risks in terms of manufacturing processes. Will the solder paste on the two pads make a different shape? Does molten solder have a surface tension that will make it pull towards the center of the combined mega-pad (and away from the components?) Are the connections more likely to fail when their pads don't have the usual well-defined borders with soldermask in between?

This will be mass produced, with pick and place machines, reflow ovens, etc. so I'm not worried about hand-soldering (although repair/rework may be more difficult with tight spacings and thermal coupling.)
I would recommend that you go to the place that is going to fab and assemble the boards for you and ask them and follow their recommendations. They may have specific experiences that lead them to recommend things that work for them that may not be in the usual set of generic guidelines.
 

kubeek

Joined Sep 20, 2005
5,654
I think your vias are ok, as they seem to be far anough from the pads, though i would move the via at Q1 just a bit left.
Vias in the middle of pads are the main issue, becasue they wick solder into them and down to the bottom layer, and so should be done with as small drill as possible and bunch more of them, rather than a few large ones.
But this again differs on the assembly, if you are doing a large powerpack by hand with no access to preheat and hot air, than a huge via in the middle of the power pad is the way to go.
 

ian field

Joined Oct 27, 2012
6,539
I would recommend that you go to the place that is going to fab and assemble the boards for you and ask them and follow their recommendations. They may have specific experiences that lead them to recommend things that work for them that may not be in the usual set of generic guidelines.
They might take one look and say: "no chance" anyway. But some will just blindly follow the drawing. Asking their advice could reveal whether they know any more than you do...…….
 

WBahn

Joined Mar 31, 2012
25,060
They might take one look and say: "no chance" anyway. But some will just blindly follow the drawing. Asking their advice could reveal whether they know any more than you do...…….
Which, in and of itself, is a very useful thing to know.

I definitely got spoiled early on because Advanced Circuits is located in the Denver area and I started getting PCB's fabbed with them not long after they started out. They knew their stuff. On a few occasions I went to their plant and sat down with their folks and worked out why something wasn't working out they way it should. I imagine that would be a lot harder to do now given how they've grown.
 
Top