Via Treatment Issues Video: Why Manufacturers Ask About Via Openings
What This Video Covers
This EQ case explains why a PCB factory pauses production when via treatment in the order, fabrication notes, emails, and Gerber solder mask layers do not describe the same result. "Covered," "open," "tented," and "resin-filled" are not interchangeable labels. They drive different mask programs, fill sequences, and surface-finish behavior on FR4 PCB and HDI PCB builds.
The video walks through four production conflicts: order-versus-Gerber cover/open mismatch; resin-filled or via-in-pad holes that still show mask windows; mixed open/tented/plugged vias on one board with no grouping rule; and large plated through-holes whose mask treatment is undefined. The takeaway is not that every via must use one process. Mixed treatment is acceptable. Ambiguous treatment is not.
Before you send a PCB prototype or PCB mass production package, confirm that order flags, notes, and mask layers agree on the intended final surface. That same package also feeds PCB assembly yield. Open barrels wick solder; undefined VIP finishes create paste voids. Request an instant PCB quote only after the five-point consistency check in this video.
Key Highlights
- CAM will not guess when the order says covered vias and the solder mask Gerber shows openings, or the reverse. Both sources can be "intentional"; only one can be released to production.
- Resin-filled and via-in-pad holes still need a defined final surface: exposed/planarized pad versus mask-covered. A mask opening over a plugged via is a process question, not a default.
- Mixed open, tented, and resin-plugged vias on one board are valid. They must be grouped in notes or a plug layer. Ambiguous mixed treatment is what stops the job.
Why Via Treatment Conflicts Trigger a CAM Engineering Query
Via treatment is specified in more places than most design packages acknowledge: the web-order checkbox, fabrication notes, email threads, a dedicated plug or via-type layer, and the top/bottom solder mask Gerbers. Each source can be internally consistent and still contradict the others. CAM cannot pick a winner without creating a board that fails either the written spec or the artwork.
The factory question is not "open or covered?" in the abstract. It is "which source is the intended manufacturing result?" Covering a via that must stay open blocks ICT probes and HASL wetting of the barrel. Opening a via that must stay tented lets solder and flux enter the hole on HASL or wave, leaves copper exposed to handling contamination, and can steal paste from nearby SMT pads.
On multilayer and HDI PCB designs the cost of the wrong call is higher. Resin plug, planarization, and copper cap are sequenced before mask. Once that sequence is locked, a leftover mask aperture cannot restore an open barrel. That is why the EQ is raised before drill and mask programs are released, not after first article.
Case 01: Covered in the Order, Open in the Gerber
This is the most common conflict. The order (or notes) says covered / tented / cover oil. The mask Gerber still carries apertures over those vias. The opposite also occurs: the order says open, the Gerber is closed.
Neither file is automatically wrong. Some CAD exports open every via by default. Some order UIs default to tenting. Designers also leave openings on test or thermal vias while intending the rest of the population to be tented. CAM cannot infer that rule from mixed artwork alone.
If the board uses HASL, an open via will take solder into the barrel. That may be desired for through-hole wetting or probe access. It is a defect if the intent was tenting to stop wicking next to fine-pitch SMT. ENIG and OSP change the cosmetic and oxidation picture, but they do not remove the need for one agreed mask state.
Recommendation: State a single rule in fabrication notes, "vias with mask openings remain open; all others tented," and make the Gerber match that rule. Do not rely on the order checkbox to override artwork, or artwork to override the order.
Case 02: Resin-Filled Vias With Mask Openings Still Present
Customers often request resin-filled vias for via-in-pad, BGA escape, or high-density stitching. The mask Gerber then still shows openings over those same holes. That is not automatically a data error. A filled, planarized via that becomes part of an SMT pad is supposed to remain solderable. A filled via that is only structural should usually be mask-covered after planarization.
The process question is the final surface, not the fill itself. Fill and planarize happen before LPI mask. If CAM follows the open Gerber, the plugged face may receive finish in a dimple or leave resin exposed. If CAM closes the window without confirmation, a pad that needed to stay solderable is tented.
| Via intent | Typical process | Mask Gerber should show | Risk if data conflicts |
|---|---|---|---|
| Signal via, away from pads | Tent / cover oil | No opening | Solder wicking or exposed copper |
| Test / probe via | Open | Opening both sides (or as noted) | Blocked ICT if tented by mistake |
| Resin plug, non-solderable | Fill + planarize + mask cover | No opening | Open window after plug; uneven mask |
| Via-in-pad (solderable) | Fill + planarize + copper cap | Opening as part of the pad | Masked pad or paste void if closed |
Case 03 and 04: Mixed Treatment and Large PTH
A single board can mix open, tented, and resin-plugged vias. CAM is not trying to force one process on every hole. The EQ appears when the mix is not defined: no via group table, no plug layer, no note that "BGA vias Type VII, stitching vias tented, test vias open." Guard vias and via fences are frequent omissions. Notes say "all vias plugged" while the designer meant only the BGA field.
Large plated through-holes raise a related mask question. A ~3.1 mm PTH with no intended mask opening still needs a defined treatment. Mask that partially enters a large hole, or that is expected to tent a diameter the LPI film cannot reliably bridge, changes how the hole finishes and how HASL or ENIG coats the barrel. Even a "simple" PTH becomes an EQ when mask intent is missing.
Five-Point Check Before You Release Gerbers
- Order requirements: Does the via-treatment flag match design intent, not the UI default?
- Solder mask layers: Are the vias that should be open actually open, and the rest closed?
- Resin plugging: Do plug scope and mask openings agree on the final surface?
- Mixed treatments: If groups differ, are they named in notes or a dedicated layer?
- Consistency: Do order, notes, emails, and Gerbers describe one result?
Do not only check "open versus covered." Check whether the manufacturing data package agrees on the intended treatment. That agreement is what lets CAM release 4 layer PCB, 6 layer PCB, and 8 layer PCB jobs without a hold, and what keeps PCB assembly from inheriting solder-steal or probe-access defects.
How Via Open vs Cover Affects Finish, Assembly, and Reliability
On HASL, open vias accept solder; tented vias are intended to keep it out. Incomplete tents on larger drills can still leave a pin-hole that fills with tin beads, a common visual and assembly complaint. On ENIG, an unexpected opening exposes nickel-gold in a location that may oxidize or take contamination during handling. On OSP, an unexpected opening changes which copper must remain solderable through storage.
For automotive PCB, aerospace PCB, and medical devices PCB programs, barrel contamination and incomplete fill are reliability items, not cosmetics. Via-in-pad on consumer electronics PCB and telecom HDI fails assembly when paste disappears into an unfilled or incorrectly finished hole. Specify IPC-4761 type when the process is more than simple tenting, and keep Gerber mask data aligned with that type.
FAQ
Q1: Why won't the factory just follow the Gerber when the order says the opposite?
A1: Because both sources are customer-controlled manufacturing data. Following Gerber against a written "cover" flag (or the reverse) produces a board that fails the other document. CAM confirms intent so the released mask program matches the functional requirement, test access, solder-wick control, or via-in-pad solderability.
Q2: Can resin-filled vias still have solder mask openings?
A2: Yes, when the filled via is planarized and intended as a solderable via-in-pad surface. No, when the fill is only to seal the barrel and the face should be mask-covered. The mask layer must state which outcome is required; an opening over a "plug and tent" note is a conflict.
Q3: Is mixed via treatment on one PCB allowed?
A3: Yes. Open test vias, tented stitching vias, and resin-filled BGA vias routinely share a panel. What is not allowed is an undefined mix. Group vias in fabrication notes or a plug/via-type layer so CAM does not apply one process to every drill.
Q4: Do large plated through-holes need a via-opening callout?
A4: If there is no SMT function, still define whether mask should open around the hole. Large diameters do not tent reliably with LPI; an undefined opening changes HASL/ENIG behavior in the barrel and can generate an EQ even on an otherwise simple PTH.
Q5: Does resolving via-opening EQs change PCB price or lead time?
A5: Unclear treatment stops CAM and adds an engineering-query cycle. Changing a population from open to resin-fill-and-cap does add process cost. Aligning Gerber and notes before order entry avoids both the hold and an unplanned process upgrade.
You asked for the vias to be covered.But your Gerber shows openings.
So which one should the factory follow?
This kind of conflict can happen when different parts of a PCB order describe the same via differently.
Via treatment can be specified in several places—your order, process notes, emails, or Gerber files.
When these sources don't match, the CAM team needs to confirm the intended result before production.
Let's look at a few real production cases.
Case 01 — Cover vs Open
This is one of the most common conflicts we see.
The order says covered, but the Gerber shows open. Both can be intentional—the Gerber may show an opening by design, while the order specifies a different manufacturing treatment.
So the CAM team needs to confirm which treatment is actually intended for production. Otherwise, the finished board may not match the intended design or process.
And the conflict can go either way—the order may say open while the Gerber shows covered.
The direction doesn't matter. What matters is that the two sources agree before production.
Case 02 — Resin-Filled, but How Should It Finish?
Here, the customer requests resin-filled vias, often for via-in-pad or high-density designs.
But the solder mask Gerber also shows openings over those vias.
This isn't necessarily a problem. In a via-in-pad design, the filled via may be planarized and finished as part of the pad.
The question is: what final surface is actually intended?
If the resin-filled via is meant to remain exposed, the manufacturing process needs to support that finish. If it should be covered by solder mask instead, the mask data needs to reflect that.
So CAM needs to confirm the intended final treatment before production.
Case 03 — Mixed Treatment
A single board can use different via treatments.Some vias can be open, while others are tented or resin-plugged.
The issue arises when the different treatments aren't clearly defined in the Gerber, fabrication notes, or other manufacturing data.
CAM is not trying to force every via on your PCB to use the same process.
Mixed treatment is fine—ambiguous treatment is not.
If different vias need different treatments, make that distinction clear in the fabrication notes or other manufacturing data.
Case 04 — Supporting Case — Large PTH
A similar issue can appear with large plated through-holes.
For example, if a plated ho le is around three point one millimeters in diameter and has no intended solder mask opening, the mask treatment may affect how the hole is finished.
So even a simple plated through-hole can raise an engineering Query when its mask treatment isn't clearly defined.
Before you release your next board package for fabrication, run through this five-point check:
Before You Release Your Gerbers
① Check your order requirements
Does the via treatment match your actual intention?
② Check the solder mask layers
Are the intended vias actually open or covered?
③ Check resin plugging requirements
Do plugging and mask openings agree?
④ Check mixed treatments
If different vias need different treatments, are they clearly defined?
⑤ Check consistency
Do your order, notes, and Gerber files agree?
Don't just check whether a via is open or covered.Check whether your manufacturing data agrees on the intended treatment.A clear, consistent data package helps CAM confirm your design intent and keep production moving.
Have a PCB project ready? Check out AIVON through the link in our profile.And don't forget to claim your new-customer offer for your first order.
