The four types
- Through: goes through the whole board. Cheapest and most common.
- Blind: connects an outer layer to an inner one without going through.
- Buried: connects inner layers only.
- Microvia: laser-drilled, small diameter, typical of HDI boards (IPC-2226); the aspect ratio is usually around 1:1.
Aspect ratio
Board thickness divided by hole diameter. The higher it is, the harder it is to plate the hole uniformly. For through vias, many fabricators work comfortably up to about 8:1 to 10:1 in a standard process; beyond that, check with your fabricator.
Annular ring and IPC class
The annular ring is the copper left around the hole. IPC-6012 defines the acceptable minimum per class: Class 2 tolerates ring breakout within limits, while Class 3 requires a minimum ring (on the order of 50 µm on outer layers and 25 µm on inner layers). In design, size the pad taking the fabricator's drill tolerance into account.
Via treatment: IPC-4761
| Type | Description |
|---|---|
| I | Tented — covered by dry film/mask |
| II | Tented and covered (mask over the film) |
| III | Plugged — partially plugged |
| IV | Plugged and covered |
| V | Filled |
| VI | Filled and covered |
| VII | Filled and capped — filled and plated over (via-in-pad) |
Via-in-pad: under fine-pitch BGAs it is often unavoidable. Specify Type VII; an open via in the pad “steals” solder and creates voids.
In Allegro X
- Create the via padstacks and list the allowed ones in Constraint Manager's Physical domain.
- For blind/buried vias, define layer pairs in Setup > B/B Via Definitions.
- Generate separate drill files per layer pair.
References and further reading
Original text for educational purposes. Menus and commands may vary between Allegro X versions; check the Cadence documentation for your version.