Technical Guidance: Five Via Finishes: Exposed, Tented, Plugged, Epoxy and Copper Paste Filled
6 min
- Definition and Universal Inspection Standards
Definition and Universal Inspection Standards
In response to customer requests, we have added the processes of "plugged vias," "epoxy-filled vias," and "copper paste filled vias," which can be selected in the ordering interface. Refer to the rules for via-in-pad filled vias (click here to view).
When ordering a PCB there are generally five via covering options available: Untented (Exposed), Tented, Plugged, Epoxy-Filled & Capped, and Copper-Paste-Filled & Capped.
| Finish Type | Appearance | Key Advantages | Key Limitations |
| Untented (Exposed) | No soldermask ink on vias | Easy post-assembly testing; some heat dissipation | Risk of solder wicking and shorts |
| Tented | Soldermask covered | Default choice; prevents solder splatter | Possible slight yellowing |
| Plugged | Ink-filled + soldermask | No solder leakage; solves yellowing | Possible minor bubbles or uneven surface |
| Epoxy-Filled & Capped | Filled + copper plated over | Flat surface; ideal for via-in-pad | Higher cost (free on 6+ layers in some cases) |
| Copper-Paste-Filled & Capped | Filled + copper plated over | High thermal conductivity (8 W/m·K) | Higher cost |
■ With exposed and tented vias, it is possible for solder beads to remain inside the hole because the hole is not completely sealed. Where this is not acceptable, filled vias should be used.
■ Vias exposed on either side of the board, via-in-pads, and vias within 0.35 mm of adjacent soldermask openings, cannot undergo ink-plugging inside the holes. Such via holes can be filled with epoxy or copper paste.
1. Exposed Vias
Definition: This option removes soldermask over all vias, exposing them to the same surface finish as all other exposed copper (HASL or ENIG depending on the selected surface finish).
Inspection Standard: Exposed via pads should be solderable both by reflow and by manual soldering.
Key Reminders:
❶ Vias differ from through-hole component pads. Untented vias are not intended for soldering components (via hole sizes are not strictly controlled, whereas component pad holes are controlled at +0.13/–0.08 mm). If components require through-hole pads, they should be designed as component pad holes with exposed solder pad openings.
❷ Most PCBs use tented vias by default. If untented vias are required, maintain at least 0.2 mm clearance from the edge of the exposed via pad to any adjacent exposed pad to prevent solder bridging during HASL (for clearances below 0.2 mm, ENIG is recommended).
2. Tented Vias
Definition: Refers to via holes where soldermask is applied, and there is no solder on the pads. This is the process used in most PCBs.
Inspection Standard: No solder should adhere to the exposed via hole solder pads after reflow soldering or hand soldering.
Key Reminders:
❶ Via holes should not be too large. Try not to exceed 0.4 mm and no larger than 0.5 mm at most for vias where allowed by wiring and current-capacity requirements. If via holes exceed 0.5 mm, there may be a risk of incomplete soldermask coverage during production, leading to the possibility of exposed via holes without ink on the hole walls. Complaints will not be accepted if poor tenting results from excessively large via holes.
❷ Slight yellowing/browning around tented via pads is a normal and inevitable outcome of the tenting process. The soldermask ink is a viscous liquid. When applied and baked in the oven (approximately 300°C), it becomes more fluid and can flow down into the hollow via hole due to the slightly raised annular ring and surface tension. This results in a thinner ink layer on the pad, allowing the copper color to show through.
3. Plugged Vias
Definition: Refers to the process of first plugging soldermask ink into the via holes using aluminum sheets, followed by full-board soldermask printing. The hole plugging rate can reach over 98% (excluding via-in-pad), completely solving the issue of via hole yellowing.
Inspection Standard: The via pad yellowing rate should be below 2%. No solder adhesion is allowed, and the opacity of the plugged holes should be 95% or higher.
4. Epoxy Filled Vias
Definition: Refers to plugging non-conductive epoxy into via holes, followed by leveling and copper plating over the pads. This process is suitable for any via with soldermask openings on one or both sides, including via-in-pads.
Inspection Standard: Completely opaque. Normal soldermask on non-exposed vias and normal HASL or ENIG on exposed vias. Hole surface copper thickness ≥ 5 μm; leveled pads show a maximum depression/protrusion within 50 μm.
5. Copper Paste Filled Vias
Definition: Refers to plugging conductive copper paste into via holes, followed by leveling and copper plating over the pads. This process is suitable for the same via types as epoxy filling.
Inspection Standard: Completely opaque. Normal soldermask on non-exposed vias and normal HASL or ENIG on exposed vias. (The advantage over regular epoxy filling is its high thermal conductivity of 8 W/m·K.) Hole surface copper thickness ≥ 5 μm; leveled pads show a maximum depression/protrusion within 50 μm.
Key Reminders:
❶ Regardless of the type of plugged holes, via hole sizes should not exceed 0.5 mm. If via holes exceed 0.5 mm, there may be cases of incomplete plugging, leading to partial transparency or yellowing of the hole openings. Complaints will not be accepted.
❷ For those requiring epoxy/copper paste filling, please illustrate which via holes need plugging, or specify the range of hole sizes that should be epoxy/copper paste plugged when placing an order.
❸ For those requiring ink plugging, please provide PCB source design files as long as possible. We will tent and plug ink for all vias that meet process requirements. If you place an order with Gerber files instead and require ink plugging for vias, please provide drawings highlighting which vias need plugging. Additionally, specify the hole size for ink plugging in the "Personalized Services" - "PCB Order Notes" when placing the order.
We will remove soldermask openings for these exposed vias and change them to tented and plugged production (strongly recommended to check "Confirm Production Files").
Q: When should I choose filled vias (plugged/epoxy/copper paste) instead of tented vias?
Use filled vias whenever solder beads inside the hole, yellowing, or via-in-pad are not acceptable.
Q: Are there any size limits for plugged vias?
Yes. All plugging processes (ink/epoxy/copper paste) require via holes ≤ 0.5 mm. Larger holes risk incomplete plugging, semi-transparency, or yellowing.
Q: What is the difference between copper paste filled vias and epoxy filled vias?
Copper paste offers high thermal conductivity (8 W/m·K), significantly better for heat dissipation. All other appearance and process requirements are identical.
Q: How do I specify which vias need special treatment when ordering?
For ink plugging, preferably upload CAD source files. With Gerber files, attach a drawing or note the hole size range in “PCB Order Notes”. For epoxy/copper paste, simply specify the required hole size range or vias in the order notes.
Keep Learning
PCBs Gold Fingers - Why It Matters ?
What is PCB Gold Finger? PCB gold fingers refer to the metal contact points on a printed circuit board, typically located at the board's edge. They are commonly made of metallic materials such as gold or upgraded gold alloys . Since the surface of the pads is gold-plated and the conductive contacts are arranged like fingers, they are called "gold fingers". Gold is extremely resistant to oxidation and has strong conductivity in comparison with other PCB surface finishes like HASL. Although it looks nic......
Technical Guidance: Five Via Finishes: Exposed, Tented, Plugged, Epoxy and Copper Paste Filled
Definition and Universal Inspection Standards In response to customer requests, we have added the processes of "plugged vias," "epoxy-filled vias," and "copper paste filled vias," which can be selected in the ordering interface. Refer to the rules for via-in-pad filled vias (click here to view). When ordering a PCB there are generally five via covering options available: Untented (Exposed), Tented, Plugged, Epoxy-Filled & Capped, and Copper-Paste-Filled & Capped. Finish Type Appearance Key Advantages ......
How to Waterproof a PCB: A Step-by-Step Potting Guide
PCBs are everywhere, they are an integral part of nowadays essential things. We can not imagine a world without them. Almost all the things which have power or that can take power have at least a PCB. Because they are used so often the circuit needs to operate in challenging environments. Mostly we are talking about outdoors, under the hood or in humid industrial settings. The term potting becomes a crucial solution for all this. Potting a printed circuit board (PCB) helps protect it from moisture, du......
HASL Surface Finish : Proven Reliability and Cost Efficiency in High-Quality PCB Manufacturing
In case you have ever been confused by seeing the acronym HASL on the PCB spec sheet and wondered what it means, here is the brief description: HASL is the abbreviation of Hot Air Solder Leveling, and it is one of the oldest, and still most dependable, surface finishes in the printed circuit board. You simply put the board into a pot of molten solder, typically a tin-lead or lead-free blend, and blow hot air over the solder to remove the excess and leaving a thin coat of solder on each exposed copper ......
Design and Surface Finish of Coil Boards
Circular coils are a wiring method sometimes used in PCB layout. They serve primarily as inductors, transformers, antennas, and more. Considering the production of PCBs containing coiled traces, please take note of the following points: 1. Compared to conventional circuits, it might not be possible to detect short circuits between windings of circular coils if the coil is a closed circuit. Therefore, the requirement for trace width and spacing is 0.254 mm (with a limit of 0.15 mm, but only when the co......
Conformal Coating in PCB Technology: Benefits, Challenges, and Future Developments
If you're searching for conformal coating, you're likely looking for a reliable way to protect your PCB from moisture, dust, chemicals, or harsh environments. Choosing the right coating directly affects product reliability, performance, and lifespan. In this guide, you'll learn what conformal coating is, the main types available, and how to select the best option for your application. We'll also cover key benefits, application methods (manual, automated, and selective), as well as inspection, rework, ......