What's so errorish on placing a via on a pad?

Go To Last Post
18 posts / 0 new
Author
Message
#1
  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Hi,

I've got a question: When using 1206 resistors in board design I place a via to the bottom layer (from the top layer) within one of the pads. The DRC says that it's an Bad Via Location. Why? What's bad about it? Seems ideal for saving space.

Thanks,

David

There are pointy haired bald people.
Time flies when you have a bad prescaler selected.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

The via can wick the solder away from the pad resulting in an unreliable joint. It is possible to have them plugged, but it's expensive. Plugged vias in pads are sometimes used on high-speed designs, to minimise inductance.

Leon

Leon Heller G1HSM

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

After all, we want the best possible solder connection so that lead does not have to be used, right? (tongue only partly in cheek).

:Jim

Jim Wagner Oregon Research Electronics, Consulting Div. Tangent, OR, USA http://www.orelectronics.net

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Will it help if the via is plugged from the other side with Solder mask?

There are pointy haired bald people.
Time flies when you have a bad prescaler selected.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

It's capillary action that draws the solder in, solder mask might not make much difference.

If the vias are small, I can't see them causing much trouble with 1206 devices. I wouldn't risk it with 0603 devices.

Leon

Leon Heller G1HSM

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

I regularly do place vias on pads of capacitors or resistors - even of IC-pins.

As already mentioned this saves pcb-space in a good way.

I can understand the disadvantage with the solder, that wicks away through the via. But it was not that difficult, as you might think now.
I never had problems with the assembly of capacitors/resistors that has vias on its pads, although it was a bit harder than assembling parts on pads without the vias.
The trick is simply to be quick while soldering. So there is not enough time for the solder to wick through the holes of the vias.

PS: I refer to simple soldering with a solder-iron. I have no clue on soldering in an alternative way.

PS: I usually place vias with a 0.4mm drill.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

I've been told that on nearly ALL commercially made circuit boards, all the holes are plated through. So every pad (atleast for a through hole part) could be a via as well.

I'm not sure why the DRC is upset though. Perhaps it assumes the hole will be plated through to both sides. Which program? EAGLE?

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Manual soldering won't be a problem, it's solder paste that would cause difficulties with vias in pads as only a thin film is used.

Vias are always plated, otherwise they wouldn't work.

Leon

Leon Heller G1HSM

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

It's for manual soldering. The program is OrCAD. It's got a bit overzaelous DRC. Reports errors like placement errors all over the board for almost all parts although there clearly are none .

There are pointy haired bald people.
Time flies when you have a bad prescaler selected.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

I sometimes send my gerber files to www.freedfm.com to get a DFM report as a double check. It has ID'd a few potential errors for me in the past.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Your pad should have enabled option "Allow via under pad".

Go to Layout Library manager, select desired component, select desired pad, click right mouse button (or Ctrl+E) and check the box "Allow via under pad". Save that component under different name (clearly marking that via under pad is enabled), to avoid problems in a future.

Gintaras

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

daqq wrote:
Will it help if the via is plugged from the other side with Solder mask?

there's no guarantee the soldermask will plug anything. surely it won't plug bigger holes.

there's yet another problem associated with holes in SMT pads when using reflow soldering. not only will there be less solder available, but more seriously, the resulting difference in forces from surface tension will pull the component toward the undrilled pad. it can even make the part stand up on that terminal. quite a good reason for not allowing such design practices by default...

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

If you're assembling it by hand I'm sure it will be ok, but I once used vias in pads for a particularly dense PCB and the assembly contractor complained bitterly that the whole run had to be retouched by hand because of solder wicking. So the rule is good, and knowing when (not) to break it is also good.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Thanks guys. I moved the vias, just to be on the safe side.

There are pointy haired bald people.
Time flies when you have a bad prescaler selected.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

leon_heller wrote:
Manual soldering won't be a problem, it's solder paste that would cause difficulties with vias in pads as only a thin film is used.

Vias are always plated, otherwise they wouldn't work.

Leon

Vias are always plated, but often holes for components (not vias) are plated too.

Thats one thing that I never knew. I thought that only vias were plated, when in fact, usually all holes are plated

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Yes, it increases reliablity if all holes are plated. Boards with non-plated vias and other holes are a lot cheaper and OK for amateur use, but assembly can be awkward. One advantage is that they can be made at home quite easily.

Leon

Leon Heller G1HSM

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

If I understand the process correctly, EVERYTHING is covered in copper (even sides from milling and such) and then it is undone.

There are pointy haired bald people.
Time flies when you have a bad prescaler selected.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

I know this thread may be a bit cold but..

I thought this white paper does a good job summarizing the key points.
http://www.techonline.com/article/pdf/showPDFinIE.jhtml?id=2010020751