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.

Vias too close to pads of the same net?

Status
Not open for further replies.

eem2am

Banned
Advanced Member level 4
Joined
Jun 22, 2008
Messages
1,179
Helped
37
Reputation
74
Reaction score
24
Trophy points
1,318
Activity points
0
Hello,

why is it that putting a via near a pad of the same net makes a board non-manufacturable?

-Also, why is it bad practice?


I have been told to re-do a double-sided layout because i have a few 0.6mm/1.2mm vias just 0.1mm away from SMD resistor pads of the same net.

...the via "restring" is not touching the pad of the resistor....as i said, it is 0.1mm away...and in any case, it's of the same net.

(-the vias are 0.6mm drill, and 1.2mm overall diameter)


So do you know why this is a bad thing?
 
Last edited:

PCB Manufacturers or companies design rules may be quite different. I also don't know the involved technology, so I can't comment the particular case. I think that either copper-to-copper or solder mask rules are affected. There's a special point with same-net copper. Basically, same net copper-to-copper spacing is not absolutely required. But some people want to have a minimum same net spacing to get separated copper etched properly, even if it's same net. Otherwise, connect it by a trace.

Other design rules are related to solder mask. There are two cases. For tented vias, you want a minimum solder mask width to keep the via protected from process chemicals. Having the via annular ring completely covered with solder mask should comply with this requirement. For open vias, a minimum solder mask strip between pad and via copper must be kept to prevent solder drain. So if the via annular ring is completely exposed, 0.1 mm copper-to-copper may be too low.
 
  • Like
Reactions: eem2am

    eem2am

    Points: 2
    Helpful Answer Positive Rating
I hhave heard complaints from PCB assembly unit about via very near to pad. They are telling while soldering ( machine process) solder/ paste is flowing out through the via and the coponent get less soldered. (the same case occured for vias on thermal pads of QFN etc)

It is better to provide a decent clearance from the SMD pad even for the same net .
 
Status
Not open for further replies.

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Back
Top