Via tenting covers a via with solder mask, plugging pushes material partly into the hole, and filling fills the hole completely, with an optional metal cap on top for vias in pads. IPC-4761 names seven via protection types for these options, from Type I (tented) to Type VII (filled and capped). Which one you need depends on how close the via is to a pad, whether it sits inside a pad, and how the board is assembled and tested. This guide explains each type, when to use it, what it changes in cost and fabrication, and how to write it in your fab notes.
1. What Do Tenting, Plugging and Filling Mean?
| Treatment | What happens to the via | Main purpose |
|---|---|---|
| Tenting | Solder mask is laid over the hole opening; the hole itself stays empty | Keep solder and paste out of the via, prevent bridges near pads |
| Plugging | Material is pushed partly into the hole from one or both sides | Seal the via more reliably than tenting alone |
| Filling | The hole is filled completely with a conductive or non-conductive material | Seal the via fully, e.g. for vias near or under pads |
| Filling and capping | The filled via is plated over with copper on both sides | Make a flat, solderable pad surface for via-in-pad |
Tenting with liquid photo-imageable (LPI) solder mask may not close every hole reliably, especially larger ones; when a via must be sealed, plugging or filling is the dependable option.
2. What Are the IPC-4761 Via Types?
IPC-4761 defines seven types (IPC training material, pp. 54–60; IPC-4761 contents, sections 5.1–5.7):
| Type | Name | What it is |
|---|---|---|
| I | Tented | Solder mask spans the hole; no material in the hole |
| II | Tented and covered | Type I plus an additional covering layer |
| III | Plugged | Material partly enters the hole |
| IV | Plugged and covered | Type III plus a covering layer |
| V | Filled | The hole is filled through its full length |
| VI | Filled and covered | Type V plus solder mask covering |
| VII | Filled and capped | Type V plus metallization (a copper cap) on both sides |
Types I–IV and VI can be applied to one side or both sides of the board. Two points are often misunderstood: Type II is not simply “tented on both sides,” and Type VI (covered with mask) is not the same as Type VII (capped with copper).
IPC-4761 is a design guide from July 2006 and is now listed by IPC as no longer maintained (IPC revision table). It names the types; the acceptance criteria for fill, voids, dimples and cap plating come from the performance specification on your order, such as IPC-6012.
3. Which Via Treatment Should You Use?
| Via situation | Usual treatment | Why |
|---|---|---|
| General vias away from pads | Type I or II (tented) | Lowest cost; keeps solder out of the via |
| Vias close to SMD or BGA pads (dog-bone fanout) | Type III/IV (plugged) or Type VI (filled and covered) | A thin mask dam can fail; sealing stops solder wicking and paste loss |
| Vias inside SMD or BGA pads (via-in-pad) | Type VII (filled and capped) | A flat, plated pad surface for paste printing and soldering |
| Vias that need test-probe access | Untented on the probe side | The probe needs exposed copper |
| Vias used for heat transfer under a thermal pad | Filled (Type V/VII) or as specified by the part maker | Stops solder draining away from the pad |
IPC’s own guidance is direct on the via-in-pad case: when via-in-pad is specified, Type VII via protection is recommended (IPC technical resource, p. 39). For BGA fanout patterns, see our guide to BGA pad design and escape routing.
4. What Goes Wrong With the Wrong Choice?
- Solder wicking: an open via in or next to a pad draws molten solder away from the joint, leaving a starved joint or a void under a BGA ball.
- Trapped chemistry: a via that is tented on one side and partly filled can trap process chemicals or air, which may outgas during reflow.
- Uneven pads: via-in-pad without a cap leaves a dimple or a hole in the pad, which affects paste volume and joint shape.
- Test access lost: tenting every via removes probe points needed for in-circuit or flying-probe test.
5. How Does Via Treatment Affect Cost and Lead Time?
Tenting adds nothing beyond normal solder mask. Plugging and filling add process steps (filling, curing and planarizing), and Type VII adds plating and another imaging step for the cap, so filled-and-capped vias are the most expensive option and add time. The amount depends on the number of holes treated, hole sizes, board thickness and the fill material, so ask for a quote with and without the treatment.
Two ways to keep cost down:
- Apply plugging or filling only to the vias that need it (for example, the BGA area), and say so in the fab notes.
- If the BGA pitch allows dog-bone fanout, avoid via-in-pad altogether; when the pitch is too fine, via-in-pad usually comes with an HDI build. Our comparison of HDI and standard PCB cost covers that decision, and our PCB fabrication cost guide covers other cost drivers.
6. How Do You Specify Via Treatment in Fab Notes?
Name the type, the side and which vias, and point to the acceptance spec:
| Item | Example note |
|---|---|
| Treatment type | “Vias marked VIP: IPC-4761 Type VII, filled and capped.” |
| Which vias | “All vias ≤ 0.3 mm finished hole, except test vias on layer X” or a separate drill file per treatment |
| Side | “Type III plugged from the secondary side” |
| Fill material | Non-conductive epoxy or conductive fill, by name if required |
| Acceptance | “Fill, dimple and cap plating per IPC-6012 Class 2” (or Class 3) |
| Test vias | “Do not tent vias in the test-point layer” |
Mark the vias in the design data rather than describing them in words only; a separate drill file or layer for each treatment removes guesswork. Our guide to Gerber files covers what to include in the fabrication package.
How Can We Help?
We do resin via plugging and plated-over capping (filled and capped vias, IPC-4761 Type VII / VIPPO), including via-in-pad on HDI and multilayer PCBs. Send your Gerber files and fab notes with the via treatment marked, and we will confirm how each via will be built and quote within 2 hours for bare boards; our free DFM check flags vias that are too close to pads for tenting alone. Our via plugging and via-in-pad options are listed in our PCB fabrication capabilities.
Conclusion
Tent vias that are away from pads, plug or fill vias that are close to pads, and fill and cap vias that sit inside pads (IPC-4761 Type VII, as IPC recommends for via-in-pad). Use the IPC-4761 type names in your fab notes, say which vias and which side, and take acceptance criteria from IPC-6012. Treat only the vias that need it to keep cost down. Contact us with your files for a quote.
FAQ
What does “tented via” mean? A via covered with solder mask so the opening is closed over; the hole itself is not filled.
Should vias be filled? Only when they need to be sealed or flat: vias in pads, vias very close to pads, or vias under thermal pads. Ordinary vias can stay tented.
How are vias plugged on a PCB? Plugging material (typically epoxy or solder mask material) is pushed into the hole from one or both sides and cured; for full filling, the hole is filled through its length and planarized.
What is VIPPO? Via-in-pad plated over: a via inside a pad that is filled and copper-capped, which is IPC-4761 Type VII.
What are the types of vias? By structure: through-hole, blind, buried and microvias. By protection: the seven IPC-4761 types above.
Upload your files today · Free DFM check before production · Ship worldwide
Get your PCB prototypes in as fast as 24 hours. We handle FR4, Rogers, and hybrid boards up to 40 layers in volume production, with advanced builds subject to engineering review — free prototypes for 2–4 layer FR-4 boards, no minimum order.
Just upload your Gerber + BOM — we source every part, assemble, and inspect (AOI + X‑Ray) so you don't have to chase suppliers. Boards ship in as fast as 24 hours.