CAM review of a high-volume 2-layer FR-4 order measuring 102 × 107 mm revealed a clear conflict between the system order parameters and the actual Gerber solder mask data. The order specified open vias, yet portions of the design files showed tented vias with cover oil. This tented via vs open via mismatch created uncertainty about the final via condition after HASL processing and directly affected manufacturing interpretation. With 1500 pieces required in a 10×6 customer panel and a one-day lead time, production could not proceed until the design intent was confirmed.
The board used standard FR-4 (KB-6165F) material with TG150 rating, 1.6 mm finished thickness, 1 oz copper on both sides, green solder mask, and white silkscreen on the top side only. Separation relied on V-cut combined with routing and zero process edge. As the final engineering checkpoint, our team examined the full data package to determine whether the mixed via treatment could be interpreted consistently for reliable fabrication and subsequent assembly.
Design Intent for Via Accessibility on Compact Boards
The project appeared to target a functional 2-layer board ( #FR4-20260211-032 ) with straightforward mechanical and electrical requirements. Minimum hole size was 0.8 mm and minimum trace/space 10 mil. The customer elected self-panelization in a dense 10×6 array. Fabrication notes and the system order indicated that vias should remain open (windowed) so that solder or test probes could access the barrels if needed. The overall design intent seemed to prioritize accessibility over complete via protection.
At the same time, the small board dimensions limited available real estate for production markings and tooling features. Fiducial marks near panel edges and proposed locating holes required careful placement to avoid interference with functional areas or separation paths. These constraints made any ambiguity in the primary solder mask data even more critical, because secondary adjustments would further reduce usable space.
The data package initially looked complete for a standard HASL job. However, layer-by-layer comparison quickly exposed the divergence between the documented via treatment and the actual Gerber geometry.
Gerber Solder Mask Data Versus System Order Parameters
Our CAM engineer first observed the discrepancy while verifying solder mask generation. The system order explicitly called for open vias, yet multiple vias in the Gerber layers carried solder mask coverage (tenting or cover oil). Further verification showed a mixed condition: some vias had clear openings while others were fully or partially tented. This tented via vs open via inconsistency could not be resolved from the available documentation alone.
Figure 1: order indicated open vias, yetthe Gerber data showed tented coverage over selected vias
The conflict immediately raised process concerns. In HASL finishing, open vias allow molten solder to enter the barrel, which can be desirable for through-hole soldering or test access. Tented vias, by contrast, are intended to prevent solder wicking and protect the barrel from contamination. A mixed or ambiguous treatment risks non-uniform results across the panel and potential assembly issues downstream.
| Engineering Observation | Conflict Identified | Potential Manufacturing Outcome | Recommended Action |
|---|---|---|---|
| System order specifies open vias | Gerber shows partial tenting | Inconsistent via condition after HASL | Confirm intended treatment |
| Small board dimensions | Limited space for cycle marks | Marking omitted or forced into functional area | Confirm if marking is required |
| Fiducial near separation path | Risk of partial cut-off | Reduced alignment accuracy | Adjust or confirm position |
Manufacturing Risks Created by Ambiguous Via Coverage
The core conflict was a data-to-data and manufacturing interpretation problem. When the system order and Gerber files diverge on PCB vias treatment, the CAM system cannot generate a single authoritative solder mask. Releasing the job without clarification would leave the factory free to interpret the mixed data either as open or tented, producing boards that differ from the customer's actual expectation.
Realistic failure scenarios included solder bridging on vias that were meant to remain open, incomplete filling of vias intended for soldering, or exposed copper on vias that required protection. Any of these outcomes could surface during electrical testing or later during customer assembly. IPC-A-600 acceptability criteria for solder mask registration and via coverage require consistency with documented design intent. Without that consistency, the design could not be considered ready for production.
The small board size amplified the importance of resolving the primary conflict quickly. Limited surface area meant that any secondary features—cycle marks, locating holes, or fiducials—had to be placed with precision. An unresolved via treatment issue would force rework of the entire solder mask generation after other features had already been finalized, increasing the chance of further errors under the one-day schedule.
Secondary Concerns of Marking Space and Tooling Placement
Supporting observations reinforced the decision to hold the job. The board dimensions left insufficient space for a standard production cycle mark without encroaching on functional copper or silkscreen. Fiducial marks positioned near the V-cut or routing path risked partial removal during separation, reducing their usefulness for downstream assembly alignment. A proposed locating hole location also required explicit customer acceptance to confirm it did not interfere with critical features.
Figure 2: the fiducial mark indicated by the arrow will be partially trimmed off
These secondary issues did not independently prevent manufacturing, yet they demonstrated that the data package still contained multiple points of ambiguity. Resolving only the via treatment while leaving marking and tooling positions open would have left residual interpretation risk.
Clarification Path and Final Manufacturing Decision
We issued a focused set of Engineering Questions. The primary question addressed the tented via vs open via discrepancy, asking the customer to confirm whether the Gerber partial tenting or the system open-window specification represented the true design intent. Additional questions covered the necessity of cycle marks given the limited board area, acceptance of the proposed locating hole position, and confirmation that fiducial marks near separation paths would remain usable after routing.
Customer response clarified that selective tenting shown in the Gerber data was intentional for specific vias, while other vias were to remain open as functional requirements dictated. Cycle marks were waived because of space constraints. Locating holes and fiducial positions were approved with minor relocation to ensure full integrity after separation. These confirmations allowed the engineering team to regenerate a consistent solder mask layer set, update the panel tooling file, and lock the marking strategy.
Figure 3: adding tooling holes at the locations indicated by the arrows
Revised manufacturing files were generated and internally verified. Solder mask expansion matched the confirmed selective tenting, open vias retained clear windows, and all tooling and fiducial features cleared the separation paths. The 10×6 panel with V-cut plus routing was confirmed manufacturable under the original one-day schedule. Only after this validation was the job released to production for the full 1500-piece quantity.
| Aspect | Before Clarification | After Resolution |
|---|---|---|
| Via Treatment | System open vs Gerber partial tenting | Selective tenting confirmed |
| Production Marking | Space insufficient for cycle | Waived by customer |
| Fiducial & Locating Holes | Risk of cut-off or interference | Positions adjusted and approved |
| Overall Readiness | On engineering hold | Released to production |
Practical Lessons for Consistent Via Solder Mask Design
- Always generate solder mask Gerber layers that exactly match the via treatment stated in the system order or fabrication notes.
- When selective tenting is required, clearly document which vias are tented and which remain open so that CAM systems can interpret the design without ambiguity.
- On small boards, evaluate available space for production markings early and explicitly waive cycle marks if necessary.
- Position fiducial marks and locating holes with adequate clearance from V-cut and routing paths to prevent partial removal.
- Cross-check system parameters against actual Gerber data before file submission to catch tented via vs open via mismatches at the design stage.
- Consider downstream assembly needs when deciding via coverage—open vias support soldering access while tented vias reduce wicking risk.
- Treat solder mask via treatment as a critical design attribute rather than a secondary detail that can be resolved later.
- Provide clear acceptance criteria for any tooling or marking features that must be added by the manufacturer on customer-panelized boards.
Conclusion
The investigation into the tented via vs open via conflict demonstrated how a single data mismatch between system parameters and Gerber layers can halt an otherwise complete high-volume order. By isolating the primary solder mask inconsistency, confirming secondary marking and tooling placements, and obtaining explicit customer direction, the engineering team converted an ambiguous data package into a manufacturable design. The final files supported consistent HASL processing and clean panel separation, allowing the 1500-piece run to meet the original one-day schedule while preserving the customer's functional requirements for via accessibility and protection.
FAQ
Q1: Why does a tented via vs open via mismatch between system order and Gerber trigger an Engineering Question?
A1: Open vias and tented vias require different solder mask generation and produce different results after HASL. Mixed or conflicting data leaves the manufacturer unable to determine the true design intent, risking non-conforming boards.
Q2: What manufacturing risks result from unresolved via coverage conflicts?
A2: Vias intended to be open may become tented and block solder or test access, while vias intended for protection may remain open and allow solder wicking or contamination. Either outcome can cause assembly defects or test failures.
Q3: How should designers document selective via tenting?
A3: Explicitly list or graphically identify which vias are tented and which remain open in the fabrication notes, and ensure the corresponding solder mask Gerber layers match that documentation exactly.
Q4: Can limited board space justify omitting production cycle marks?
A4: Yes. When the board is too small to accommodate a cycle mark without compromising functional features, the manufacturer may waive the mark after customer confirmation.
Q5: Why do fiducial marks near V-cut or routing paths require confirmation?
A5: Separation processes can partially remove marks placed too close to the edge, reducing their effectiveness for downstream alignment and potentially creating incomplete copper features.
Q6: What is the most effective way to prevent tented via vs open via conflicts?
A6: Generate solder mask layers from the same source as the fabrication notes, perform a visual cross-check before submission, and use consistent terminology (tented/cover oil versus open/window) across all documentation.
