New Posts  All Forums:Forum Nav:

Vias on SMT pads

post #1 of 15
11/9/09 at 4:02pm
Thread Starter 
Just curious, what are your opinions of vias located on smt pads? Good? Bad? who cares? The packages in question are 14 and 16 pin SOIC packages and perhaps 1206 resistor pads. The hole diameter of the via would be 15 mil and the annular ring 25 mil. Is solder stealing really an issue, or does it more depend on where on the pad the via is located? In the case of SOIC packages, is on the near the body of the component more preferable to the outside?
Reply
post #2 of 15
11/9/09 at 4:26pm
For the GrubDAC, I put the via's on the SMT pads, but not under. The are 15mil drill with 29mil ring. They were placed in such a way that the edge of the drill hole was right on the edge of the pad. I don't know if I'd put that size via under a pad. Maybe it is just me, but my soldering is not that good to ensure that it would be down properly.

As for which end of a pad to place the via, I kept them to the outside edge in general unless there was a routing reason to put them elsewhere.
Reply
post #3 of 15
11/9/09 at 8:17pm
The "solder stealing" is really only an issue if you're using solder-paste in a production environment. If you're hand-soldering with wire-solder, it doesn't matter at all. The only case when it's annoying hand-soldering is when it's in a tiny pad (0603, 0402, etc.) and connects directly to a huge ground-plane on an inner layer or something. Then it's hard to get enough heat to get the solder to flow well. That's my opinion anyways.
Reply
post #4 of 15
11/10/09 at 6:46am
Quote:
Originally Posted by Fixz8 View Post
The "solder stealing" is really only an issue if you're using solder-paste in a production environment. If you're hand-soldering with wire-solder, it doesn't matter at all. The only case when it's annoying hand-soldering is when it's in a tiny pad (0603, 0402, etc.) and connects directly to a huge ground-plane on an inner layer or something. Then it's hard to get enough heat to get the solder to flow well. That's my opinion anyways.
I second that. I do a lot of SMD stuff (as a hobby). Putting vias in pads is only a problem if you use solder paste or if the parts are too small (0603 and smaller). They tend to tombstone. They stand up and end up anooingly vertical - hard to handle.
Sparkfun has a nice tutorial on how to cover vias with solder mask to give a cleaner look.
The guys over at screaming circuits really hate vias in pads. But they explain very good their reasons (which apply only in professional production environment).

I personally put the vias always in the middle of the pad or under the pad to hide them a bit. But in the end I do not think that this really matters - apart from aesthetics
Reply
post #5 of 15
11/11/09 at 9:28am
I've done "via in pad" technology. My most complex board was a board with a BGA containing over 200 balls. Each ball went to a pad which had vias. To keep the solder from filling the holes, I had all of the holes silver filled, then their ends sanded down. This is also done using conductive epoxy (high temperature) if the cost of silver is too great.

Some boards I've assembled for people have had vias in pads without being filled. It was only a problem on a board where I had to stuff 0201 components. The solder kept going right through the PCB (which was only 5-mil thick) and the 0201 went unsoldered. To get the component to stick to the board, I turned the iron temp down to something in the area of 580F and things worked out well from there on out.
Reply
post #6 of 15
11/11/09 at 10:32am
Quote:
Originally Posted by deltaydeltax View Post
I've done "via in pad" technology. My most complex board was a board with a BGA containing over 200 balls. Each ball went to a pad which had vias. To keep the solder from filling the holes, I had all of the holes silver filled, then their ends sanded down. This is also done using conductive epoxy (high temperature) if the cost of silver is too great.

Some boards I've assembled for people have had vias in pads without being filled. It was only a problem on a board where I had to stuff 0201 components. The solder kept going right through the PCB (which was only 5-mil thick) and the 0201 went unsoldered. To get the component to stick to the board, I turned the iron temp down to something in the area of 580F and things worked out well from there on out.
The guys over at screaming circuits suggest putting some solder mask over the vias. Makes perfectly sens to me. Sounds easier than your method.
But I have not figured it out yet how to do it in eagle CAD - since there you define what to leave out of the solder mask.
Reply
post #7 of 15
11/11/09 at 10:35am
Quote:
Originally Posted by _atari_ View Post
But I have not figured it out yet how to do it in eagle CAD - since there you define what to leave out of the solder mask.
The SparkFun link you had earlier tells you have to do it in Eagle.

Now if only I could figure out how to do it in Ultiboard...
Reply
post #8 of 15
11/11/09 at 11:10am
Quote:
Originally Posted by cobaltmute View Post
The SparkFun link you had earlier tells you have to do it in Eagle.

Now if only I could figure out how to do it in Ultiboard...
Yes and no. It works for vias outside of pads. But not inside of pads. Because there you already have 'no sodlermask here' marking. But getting the soldermask back is not that easy.

Nevertheless you only need it for complicated stuff anyway. And I count BGA on 4 layer boards to that category

BTW: we need more SMT in DIY Audio
Reply
post #9 of 15
11/11/09 at 11:21am
Thread Starter 
Quote:
Originally Posted by cobaltmute View Post
The SparkFun link you had earlier tells you have to do it in Eagle.

Now if only I could figure out how to do it in Ultiboard...
heh read that yesterday as well. It's a single check box in Diptrace, so I'll probably give it a go.

Thanks guys!
Reply
post #10 of 15
11/11/09 at 11:37am
Quote:
Originally Posted by _atari_ View Post
BTW: we need more SMT in DIY Audio
I'd say yes and no.

No - I find it a pain to get a good solder joint against a ground plane for SMT.

Yes - It is so nice to be able to place and solder without flipping the board. Rs and Cs are so easy to place in 1206 size.

Something like a Dynalo in SMT should be pretty achievable.
Reply
post #11 of 15
11/11/09 at 11:39am
Thread Starter 
Quote:
Originally Posted by cobaltmute View Post
No - I find it a pain to get a good solder joint against a ground plane for SMT.
Do you notice whether or not these pads use direct thermals?
Reply
post #12 of 15
11/11/09 at 12:24pm
Thermals as in thermal relief? Yup there is thermal relief there so the whole pad isn't directly connected to the plane.

As an example, take a look at the top side of the GrubDAC (I'm not going to repost the picture here) - C4 and C11. I always find I do a better job soldering down the non-ground end first and then doing the ground side.
Reply
post #13 of 15
11/11/09 at 10:44pm
Quote:
Originally Posted by _atari_ View Post
The guys over at screaming circuits suggest putting some solder mask over the vias. Makes perfectly sens to me. Sounds easier than your method.
But I have not figured it out yet how to do it in eagle CAD - since there you define what to leave out of the solder mask.
I can say with absolute certainty, stretching solder mask over pads with vias in them will never allow you to solder to the pads, thereby making them useless. Unless you plan on scraping the solder masking material off of the pad you were trying to put a via in and opening up the hole once again (unless you were lucky enough for the solder mask to actually fill the hole. I stand by my method. Screaming circuits also mentions the method I used:

A lot of fab houses will epoxy fill your vias these days. Even micro-vias. And, yes, you should even have your micro vias filled and plated. Especially with small BGAs. It's just not worth all the risks that come along with it.

This risks are true. One set of boards actually were scrapped. The silver which was filling the vias leaked to the board's inner layers and caused numerous shorts. It's not a hard thing to have done. You write in your notes table at the top left of your assembly drawing what you want done. It's usually something like,
Notes:
1. Boards to meet IPCXXXX spec
2. Green solder resist
3. White legend
4. UL marking symbol in location marked by XXXX
5. All 8-mil vias to be silver filled and sanded
6. other notes,
7. other noes.
8........
Reply
post #14 of 15
11/12/09 at 4:29am
You are right. Solder masked vias in small pads DO NOT work.
But honestly I think that your are much more experienced her as I am.

But just as an conclusion i think:

For everything bigger than 0603 vias in pads are fine as long as you solder by hand.
For 0603 vias in pads are doable, but look ugly and can lead to problems.
For everything smaller than 0603 it WILL lead to problems.

Vias in chip-pads are only doable for SOIC - since else the pitch of the pads (speak it out loud - sounds nice) is too narrow.

So, back to tinkering
Reply
post #15 of 15
11/14/09 at 4:08pm
Quote:
Originally Posted by cobaltmute View Post
The SparkFun link you had earlier tells you have to do it in Eagle.

Now if only I could figure out how to do it in Ultiboard...


Maybe I should look harder next time.

Select the via, and then uncheck the "Soldermask Top" or "Soldermask Bottom" box.

D'oh.
Reply
New Posts  All Forums:Forum Nav:
  Return Home