Coupons
Help
  • FAQ
    browse most common questions
  • Live Chat
    talk with our online service
  • Email
    contact your dedicated sales:

Optimizing Stackup and Spacing in a 4-Layer 1-Order HDI PCB

Author : Alex Chen | PCB Design & High-Speed Engineering Specialist

November 13, 2026


During CAM preparation of a 4-layer HDI order classified as 1-order, our team identified a series of process and spacing conflicts that required customer confirmation. The board measures 110 mm by 131 mm, uses Kingboard KB-6165F FR-4 with TG150, is specified at 1.0 mm finished thickness with 1 oz copper, carries matte-black solder mask and white silkscreen, and is delivered as a customer self-panel in a 6×8 array separated by routing. Blind and buried vias are indicated, the minimum hole size is 0.15 mm, aluminum via plugging is listed, and the surface finish is immersion gold at 2U". The customer note requests production according to the Layer Stack Manager file and resin fill with capping for all vias that land on pads. These parameters establish a 1-order HDI construction in which the sequential lamination must support laser drilling while numerous local spacings fall below the limits for solder-mask bridges and routing webs.

The main engineering items included an adjustment to the customer stackup because the prepreg was too thick for laser penetration, multiple proposals for full solder-mask openings or pad shaving where pad, BGA, or slot spacing was too tight to retain bridges, reduction of certain slot lengths, deletion of stamp holes and selected break-away bridges, addition of process-edge copper and tooling holes with corner chamfers, and local compensation plus pad shaving on inconsistent via pads. Each change was illustrated and submitted for confirmation.

 

1-Order HDI Stackup Adjustment for Laser Drilling

The lamination specified in the order showed prepreg thickness too great for the laser to drill through. We adjusted the stackup and requested confirmation. In a 1-order HDI ( #HDI-20251206-0038 ) the blind vias are laser-drilled after the first lamination; the dielectric thickness above the target layer must lie within the laser ablation window. Excess prepreg prevents complete penetration, leaving residual dielectric that blocks plating and creates open circuits.

The order form indicates a customer-defined stackup and a 0.15 mm hole size, while the customer note emphasizes adherence to the Layer Stack Manager file. The adjustment therefore preserves the overall 1.0 mm thickness and 1 oz copper weights while reducing the critical dielectric to a laser-compatible gauge. Because aluminum plugging is listed yet the note requests resin fill and capping for vias on pads, the revised dielectric must still accept whichever fill method is finally confirmed. Acceptance of the adjusted stackup locks the sequential press cycle and the laser program before the sub-composite is drilled.

The current PP thickness is too great for laser ablation.

Figure 1: The current PP thickness is too great for laser ablation.

 

Full Solder-Mask Openings for Tight-Pitch Features

Several regions exhibited pad or slot spacing too small to retain solder-mask bridges. We proposed full open windows at the tight pad areas, at the board-edge slots, and at the BGA (accepting missing bridges), and requested confirmation for each. Matte-black solder mask requires a minimum web width to survive imaging, development, and registration; when the copper-to-copper gap falls below that width the web either fails to form or breaks, leaving an uncontrolled opening.

For the tight BGA pitch, solder mask bridges may be omitted where necessary.

Figure 2: For the tight BGA pitch, solder mask bridges may be omitted where necessary.

A full open window clears the entire local zone of mask, ensuring every pad or slot edge is exposed and eliminating residual filaments that could cause solder bridging or interfere with connector insertion. The same approach was applied to the edge slots whose spacing likewise prevented bridge formation. For the BGA the proposal explicitly accepts the absence of bridges. Because the order already specifies matte-black mask and the general trace/space is 3 mil, the full openings remain within registration capability while removing the process risk. Confirmation of each open-window location finalizes the mask artwork for those features.

The pad pitch is narrow. The continuous solder mask opening over the pad area is acceptable.

Figure 3: The pad pitch is narrow. The continuous solder mask opening over the pad area is acceptable.

Pad Shaving for Solder-Mask Bridges and Copper Clearance

In other locations the pad spacing was small but a bridge was still desired. We proposed shaving the pads to create sufficient gap for a solder-mask bridge and requested confirmation. A parallel note addressed inconsistent via pads that had been circled: compensation was added and the pads were shaved to guarantee a safety distance. Shaving reduces the copper diameter just enough to restore the minimum mask web without removing the annular ring needed for plating or soldering.

On a board with 1 oz copper and immersion gold, the shaved edge must remain robust after etch and surface finish. The compensation on the via pads accounts for the plating and etch tolerances so that the final copper-to-copper clearance still supports the bridge. These local modifications leave the majority of the circuitry unchanged while resolving only the features that violated mask or clearance rules. Acceptance of the shaved geometries locks the copper artwork before imaging.

 This pad is a via pad, and we need to add compensation and reduce the pad size to ensure a safe spacing.

Figure 4: This pad is a via pad, and we need to add compensation and reduce the pad size to ensure a safe spacing. 

The pad pitch is narrow. Solder mask bridge formation by pad reduction is acceptable.

Figure 5: The pad pitch is narrow. Solder mask bridge formation by pad reduction is acceptable. 

Slot Optimization and Stamp-Hole Removal for Routing

Two arrowed slot holes measured 0.4 mm by 0.6 mm and were spaced too closely to allow a solder-mask bridge. We proposed shortening the slot length to 0.4 mm by 0.56 mm so that a bridge could be formed, and requested confirmation. In a separate area the routing-slot spacing was too small to retain break-away bridges; we recommended routing the slots fully out, deleting the local stamp holes (as shown on the production GKO layer), and confirming the change. A further note highlighted additional routing whose spacing prevented bridges and suggested deleting the highlighted stamp holes and bridges while retaining only two break-away locations; a revised panel drawing was attached.

The router slot spacing is narrow.

Figure 6: The router slot spacing is narrow. 

We propose reducing the slot length from 0.4 × 0.6 mm to 0.4 × 0.56 mm.

Figure 7: We propose reducing the slot length from 0.4 × 0.6 mm to 0.4 × 0.56 mm. 

Shortening the slot restores mask-web width without eliminating the slot function. Deleting stamp holes and selected bridges where spacing is inadequate prevents incomplete webs that could tear unpredictably during depanelization of the 6×8 array. The retained two bridges provide controlled separation while the fully routed slots ensure clean edges. Because the order specifies routing separation and customer self-panelization, these adjustments refine the break-away scheme rather than alter the array count. Confirmation of the shortened slots, deleted stamps, and revised panel outline finalizes the mechanical programs.

Due to narrow slot spacing, a common solder mask opening over the slot area is required.

Figure 8: Due to narrow slot spacing, a common solder mask opening over the slot area is required.

 

Process-Edge Design: Copper Pour, Tooling Holes, and Chamfers

To facilitate production we added copper pour on the process edge, inserted tooling holes, and allowed chamfers on the four corners, requesting confirmation. Although the order lists no process edge, a temporary copper border and tooling features improve plating-current distribution and panel handling for a 6×8 array of 1-order HDI boards. The chamfers reduce sharp-corner stress during routing and handling. These additions lie outside the customer circuit outline and are removed with the process edge or routing, so they do not affect the finished 110 mm by 131 mm boards. Acceptance permits the working panel to include the copper, holes, and chamfers while the functional artwork remains unchanged.

 Added copper pours and tooling holes in the rails, with corner chamfering allowed.

Figure 9: Added copper pours and tooling holes in the rails, with corner chamfering allowed. 

Break-Away Bridge Optimization for Reliable Depanelization

The original break-away bridges were too small. We optimized their geometry and requested confirmation. Undersized bridges on a routed panel can fracture prematurely or leave excessive burrs; enlarging or reshaping them within the available spacing improves depanelization consistency for the 6×8 array. The optimization is local to the bridge features already under discussion in the stamp-hole and routing notes, ensuring that the retained bridges meet process minimums. Confirmation of the optimized bridges completes the mechanical separation scheme.

 the narrow spacing

Figure 10: the narrow spacing

Key CAM Adjustments for 4-Layer HDI Manufacturing

The items in the main engineering query address the practical limits of producing this 4-layer 1-order HDI board to the customer stackup and panel format. The prepreg thickness was reduced so that laser drilling of the blind vias can succeed. Multiple tight spacings at pads, BGA, and slots were resolved either by full mask openings or by pad shaving and slot-length reduction that restore bridge capability. Stamp holes and excess bridges were deleted where spacing prevented reliable webs, while process-edge copper, tooling holes, and chamfers were added for manufacturability. Via-pad compensation and bridge optimization completed the local copper and mechanical refinements.

Each proposal requires explicit customer confirmation because it modifies the stackup dielectric, mask openings, copper outlines, slot dimensions, or panel break-away features relative to the original data. The customer note’s request for resin fill and capping of vias on pads remains compatible with these changes once the fill method is aligned with the aluminum-plug listing. Once the adjusted stackup, mask treatments, shaved pads, shortened slots, deleted stamps, process-edge features, and optimized bridges are accepted, the laser program, mask artwork, copper films, and routing paths can be frozen. The board can then proceed through sequential lamination, laser drilling, via filling, outer-layer processing, and mechanical forming of the 6×8 panel. The case shows how CAM review of a 1-order HDI with a customer-defined stackup and dense local features commonly generates a coordinated set of dielectric, mask, copper, and panel adjustments that together bring the design inside laser, solder-mask, and routing capability.

Alex Chen | PCB Design & High-Speed Engineering Specialist Alex Chen | PCB Design & High-Speed Engineering Specialist

Alex Chen is a senior PCB design engineer with extensive experience in high-speed and high-density circuit design. He specializes in signal integrity, impedance control, and multilayer PCB layout optimization. At AIVON, he reviews and refines content related to PCB design principles, EDA tools, and advanced layout techniques. His expertise helps engineers avoid common design pitfalls and improve performance, reliability, and manufacturability in complex PCB projects.

Related Tags


2026 AIVON.COM All Rights Reserved
Intellectual Property Rights | Terms of Service | Privacy Policy | Refund Policy