The plating has a finite thickness
Because of the cooper that is inside the Via.
The PCB manufacturer drill the via a bit bigger than the specified “Via Hole size”. Together with the copper you will get the specified “Via Hole Size”
I see a gold ring surrounded by a yellow ring surrounded by a green ring, in order of increasing diameters. I understand that the drill will drill out a hole of diameter B, show by the black dotted circle.
I understand that the inner gold ring is the plated part of “plated through-hole” (added after drilling the hole). I understand that the green ring is just the extent of solder mask that will surround the hole.
I deduce that the yellow ring is just that part of the PCB between the plating and the solder mask, which is unprocessed. ( I think this part of the PCB is called “the courtyard”.) Do I understand this correctly ?
Almost
The light yellow ring (dia C) isn’t part of the plating and soldermask, this is the plating. This is the annular ring. There must always be some copper that the fabricator drills through.
There will not be any courtyard here. Courtyard is a safety border around components to ensure that a card can be populated because if components are too close they cannot be placed. Via’s do not have courtyards as they are fabricated not assembled
1 Like
I further deduce that at the board’s surface, the plating extends farther away from the drill centerline than it does below the board’s surface.
Thank you, Naib.
Exactly.
The Via is meant to route signals to other layers via a piece of copper 
There are two key pieces of information when creating a via
- Annular ring
- Via diameter
When a PCB is made it goes through a few steps
- Print your artwork onto the copper laminate
- Etch the copper laminate to leave behind your desired shapes. Repeat for all layers
- Bond all layers together
- DRILL plated holes
- PLATE
- DRILL non-plated holes
- apply mask
- apply silkscreen
Now because a via is plated with copper, the drill must be larger than the finished via (NOTE: always quote finished diameter to a fab house). So since the drill diameter > hole diameter, the starting circular shape on the PCB must be larger than the drill bit used. Not only that, drilling is not perfect (damn accurate but not perfect) and the drill is never exactly centre to the starting circular shape. This is why the “Annular ring” (because what is left after drilling is a ring) must always be larger than not only the finished via, but also their drill size. This is also why it is always recommended to include TEARDROPS on PTH to ensure that if a misalign occurs, it does not break contact with any traces leaving a via
Sounds complicated. Your 3-D picture helps, Naib. It seems to imply that even if a via is routed to copper plane y, it might NOT be connected to plane y electrically, depending on how the manufacturer processes the PCB. That is certainly an important thing to know for the person who populates the PCB.
EDIT:
The photographs showing how EAGLE makes teardrop shapes at vias is important and helpful. Thank you, Naib. Now I understand why teardrop shapes at vias is important and helpful.
No. It’s dependent on your design file. What Naib shows is a multi-layer PCB where you don’t necessarily want to connect every layer through a via, although the via passes through all layers. That’s what the “anti-pad” means. But it’s defined in your design file and has nothing to do with manufacturer processing.
The other way of solving this issue is using “buried vias”, but that’s significantly more expensive.
By “design file”, do you mean the PCB file created by Pcbnew ?
Yes, or more precisely the gerbers that are generated by pcbnew from your pcb file.
1 Like
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.