Via tenting, plugging and filling explained: IPC-4761 types
Why the via finish is a separate decision
Every via ends up in one of a few states at the fab: left open, covered by solder mask, closed with a plug, or completely filled. The layout tool only shows a drill hit and a copper ring. What happens to the hole is a process choice, and each fab offers different options and size limits.
It matters for three practical reasons:
- Solder wicking. An open via next to a pad, or inside a pad, can pull solder away from the joint during reflow.
- Shorts and contamination. Exposed via copper can bridge to a nearby component, and open barrels can trap flux, plating chemistry or solder balls.
- Assembly. Vacuum pick-up during assembly needs closed holes to hold the board.
The names are used loosely between fabs. IPC-4761 gives them fixed meanings, so use its terms in your fab notes.
The seven IPC-4761 types
IPC-4761, Design Guide for Protection of Printed Board Via Structures, was published in July 2006. Section 5 defines seven via protection types. The suffix a means the treatment is applied on one side, b means both sides.
| Type | IPC-4761 name | What is physically there |
|---|---|---|
| I | Tented via | Hole covered by a film of mask, barrel left hollow |
| II | Tented and covered via | Tent plus an additional covering of solder resist |
| III | Plugged via | Hole partly closed with a non-conductive material, no mask on top |
| IV | Plugged and covered via | Plug, then solder mask over it |
| V | Filled via | Barrel fully filled with non-conductive paste, no cover |
| VI | Filled and covered via | Filled, then covered with solder mask |
| VII | Filled and capped via | Filled, then sealed with a plated copper cap |
In practice there are three families.
Tenting (I and II) only bridges the opening. The barrel stays empty. It is cheap, but the mask can break over larger holes or leave a small gap.
Plugging (III and IV) pushes material into the hole from one side, but it does not guarantee a full barrel. Air or process chemistry can stay trapped behind the plug.
Filling (V to VII) fills the barrel completely, normally with a non-conductive resin. Type VII adds a copper cap, so you can place a pad directly on top. That is "via in pad".
What the fabs offer
From each manufacturer's own pages, checked today:
| Fab | Tenting | Plugging | Filling |
|---|---|---|---|
| EU Eurocircuits | Only together with via filling | Not used | Type VII only, resin, 0.10 to 0.50 mm finished hole |
| EU LeitOn | No longer offered | Offered (III, IV) | Offered (V to VII) |
| CN JLCPCB | Default, ideally 0.4 mm or less, 0.5 mm maximum | Mask ink plug, 0.5 mm or less | Epoxy or copper filled and capped, 0.5 mm or less |
| EU Würth Elektronik | Types I and II described | Type III with defined mask openings | Type VII, aspect ratio 1:10 or 1:8 by thickness |
Eurocircuits: no tenting without filling
Eurocircuits applies its solder mask with a spray coating process. Its soldermask guideline says this mask is not suitable for tented vias because there will always be a small opening on the hole, and ink inside the barrel can leave residue that causes adhesion and plating problems. So by default it opens every hole (PTH, NPTH and vias) free of mask. If your data has no opening for a hole, it creates one equal to the drill tool size.
To get covered vias you select "Via Filling with Resin" in the configurator and generate the mask layer without openings for those vias. The filling itself is always IPC-4761 Type VII. Eurocircuits states it only uses filling because it has more advantages than plugging, and that via filling with solder mask was discontinued in July 2020. The published limits:
- Drill tool size 0.20 to 0.60 mm, finished hole 0.10 to 0.50 mm.
- Board thickness 1.00 to 2.40 mm.
- Plated through holes only. Blind vias cannot be filled.
- At least 60% of the hole volume filled, per IPC-A-600 and IPC-6012 Class 2.
The preferred way to fill only some vias is a separate drill file or layer containing just those vias, clearly named (for example "Via Filling").
JLCPCB: five options and a size cut off at 0.5 mm
JLCPCB lists untented, tented, plugged, epoxy filled and capped, and copper filled and capped. The numbers that matter:
- Tented: vias ideally 0.4 mm or less and no larger than 0.5 mm. Larger vias are not guaranteed to be fully covered, and JLCPCB does not accept complaints about that defect.
- Untented: the via gets the same surface finish as the pads. Keep bare vias at least 0.2 mm from other exposed copper with HASL, or use ENIG for tighter spacing.
- Plugged: solder mask ink pushed into the via, then the whole board is masked. JLCPCB quotes a plugging rate above 98% (vias in pad excluded) for holes of 0.5 mm or less. Vias in pads and vias closer than 0.35 mm to a through hole pad cannot be ink plugged and need epoxy or copper filling.
- Epoxy or copper filled and capped: both for vias of 0.5 mm or less, both suitable for via in pad. The help page lists resin filling as free on boards of 6 layers and up.
Würth Elektronik: the numbers behind plugging
A Würth Elektronik CBT webinar on plugging, filling and tenting (in German) gives a useful set of design values. For Type III plugged vias it recommends these mask openings:
| Drill | Mask opening |
|---|---|
| 0.30 mm or less | 0.40 mm |
| 0.40 mm or less | 0.50 mm |
| 0.45 to 0.70 mm | drill + 0.20 mm |
| up to 0.80 mm | drill + 0.30 mm |
It also asks for 0.15 mm mask clearance to neighbouring solderable areas on both sides, notes that a plug can stand up to 70 µm above the mask, and states that Type III is not compatible with via in pad. For Type VII filled and capped vias, boards from 0.65 to 1.60 mm allow an aspect ratio of 1:10 with a smallest drill of 0.25 mm, and boards from 1.60 to 3.20 mm allow 1:8.
One sided treatment is the risky one
NCAB recommends IPC-4761 Type VI (filled and covered, aiming for complete fill) for standard products and advises against single sided plugging, including Type II, because chemistry can be trapped in the hole. It adds that solder balls are more likely with HASL. LeitOn warns that air trapped behind a plug can burst during soldering and says plugged vias should not sit under components.
Which one to ask for
Based on what the fabs above publish:
- General routing vias on a prototype. Take the fab's default. At JLCPCB that is tenting, at Eurocircuits it is open vias with surface finish. Both are fine for most boards.
- Vias close to SMD pads. Tenting stops solder wicking only if the tent holds. Keep the via drill at 0.4 mm or less if you rely on it, or move the via further away.
- Vias under a QFN thermal pad or in BGA pads. This is via in pad, and it needs Type VII filled and capped. Plugging and tenting are not via in pad options at any of the fabs above.
- Boards for vacuum handling or high reliability. Ask for filled vias (Type VI or VII) rather than tents or one sided plugs.
Whatever you pick, write the IPC-4761 type in the order notes. "Tented" alone can mean Type I, Type II or just "no mask opening" depending on who reads it.
Setting it up in KiCad
In KiCad 10, Board Setup, Solder Mask/Paste has a Tent vias setting that controls whether vias are covered with mask on the top and bottom layers. Individual vias can override it in their properties. Per via, the Properties panel lists Tented, Covered, Plugged and Filled. According to a KiCad developer on the KiCad forum, plugged and filled vias are carried in the ODB++ and IPC-2581 exports.
Gerber and Excellon do not carry a "fill this via" instruction by themselves. If you send Gerbers, the fab only sees whether the mask layer has an opening over the via. So for plugged or filled vias, add a separate drill file for those holes as Eurocircuits asks, and state the type in the order notes. Our guide to Excellon drill files explains how KiCad splits drill output, and the comparison of Gerber X2, ODB++ and IPC-2581 covers the formats that carry more information.
Check the mask layer before you order
The quickest test is visual. Open the ZIP in the PCB Tools Gerber viewer, turn on the drill and solder mask layers, and look at the vias:
- A tented via should have no mask opening at all. If you see a ring of exposed copper, the tent setting did not make it into the output.
- For Eurocircuits filling, the filled vias must have no mask openings, or they will be left open.
- Untented vias near pads need enough mask dam between them (see mask expansion and dams).
Then run through the checklist for Gerber files before ordering, and if the surface finish is still open, see HASL, ENIG or OSP, since HASL also affects how untented vias behave.
The online Gerber viewer shows the mask layer on its own, so you can see which vias have an opening before the order goes out.
Sources
- IPC, IPC-4761 Design Guide for Protection of Printed Board Via Structures (preview)
- Eurocircuits, PCB design guidelines: via filling
- Eurocircuits, PCB design guidelines: soldermask
- JLCPCB, PCB via covering
- LeitOn, Via plugging, tenting and filling (IPC-4761)
- Würth Elektronik, Webinar: Plugging, Filling, Tenting (German, PDF)
- NCAB Group, What type of via hole plugging is recommended?
- KiCad, PCB Editor manual (10.0)
- KiCad forum, Filled via request
Information in this article comes from the public documentation of manufacturers, standards bodies and software vendors as of the publication date and may have changed. Check current conditions with the company concerned before you order. Company and product names are trademarks of their owners; mentions are editorial, with no sponsorship or affiliate relationship. See the terms of use.
Check your Gerbers before you order
Load the ZIP or RAR your EDA tool exported and inspect every layer, drill and outline in the browser. Free, no account.
Open the Gerber viewer