Continue to Site

Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

Register Log in

Vias close to same net pads...how near can they be?

Status
Not open for further replies.
T

treez

Guest
Newbie level 1
Hello,

I have round vias which are drill=0.6mm, and overall diameter = 1.2mm.

In many cases i have the via "just touching" the pad of a "same net" pad. (the via is actualy connected to the pad)

..is this ok?

...i have heard rumours that the nearby via can "****" solder off the pads and cause components to be improperly soldered.
 

This is a similar situation to via-in-pad. The attachment has some suggestions to prevent the solder from running down the via.
 

Attachments

  • Screaming Circuits - Via In Pad Guidelines.pdf
    190.6 KB · Views: 156
  • Like
Reactions: treez

    T

    Points: 2
    Helpful Answer Positive Rating
I would say no, You would result in a "huge" area opened in the soldermask, and if, if they misplace this could be a problem. Furthermore You need a wide trace between pad and via to aviod sharp edges called acid traps.
 
  • Like
Reactions: treez

    T

    Points: 2
    Helpful Answer Positive Rating
Ideally - doing this is not a good idea, as said it can cause acid traps - it can also (on small 2 terminal components) if on one side only cause a thermal imbalance as the heat wicks into the via cooling the pad - but many assemblers can manage this with the right profiles etc.

The old rule of thumb is to have the via 10 thou from the pad.

It's all about making compromises, we have our ideals situations and then the real ones that make us break little rules of thumb to get the job done, the final decision is upto you but if you can design the board without breaking the rules then it is best done so.
 

To refer to the problem mentioned in the original post, I agree that via opening should be separated from the pad copper by solder resist for regular vias. The most simple solution is a modified via padstack, with a smaller solder resist opening, e.g. 0.8 mm in the said case.

The "acid trap" problem mentioned by Mattylad remains. Another problem is that PCB manufacturer design rule checks are often performed in a simplified manner, without generating (or importing) full net list information. They can't determine same net property for copper features that aren't connected on the checked layer. In both regards, connecting via copper and pad with a track of sufficient width would help.
 

Thanks

They can't determine same net property for copper features that aren't connected on the checked layer. In both regards, connecting via copper and pad with a track of sufficient width would help.
Click to expand...

....i agree with this, but that creates another question because no PCB package on earth seems to like doing this.....they all seem to delete the extra track with their "ring removal" feature.

you can disable the "ring removal" feature, but its inevitabel that you will need it enabled for other areas of the board, and so you end up enabling it again, and the blessed track that was added to the via disappears.
 

Status
Not open for further replies.

Similar threads

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Back
Top