6-Layer PCB Stackup: How to Assign Signal, Ground, and Power Layers

Four green PCB units on a panel, viewed from above.

GEMTECH PCB

For a 6-layer PCB stackup, start with the main constraint in the existing four-layer layout: insufficient signal-routing space, reference planes that do not suit critical nets, or too little copper area for power. Assign the two added copper layers to those needs, then check reference paths, dielectric spacing, and materials. The role of each layer depends on the selected stackup, so total board thickness or layer count alone does not determine suitability.

Adding two layers: which bottleneck should they solve?

Before adding two layers, identify what the four-layer board cannot accommodate. If signal routing is the main constraint, add a signal layer. If critical nets need a more suitable copper reference, evaluate an added ground reference layer. If the copper area for power is insufficient, reserve a power layer or a copper region for power.

Record the layer and reference plane for each critical net, and note how the power nets are distributed. If the four-layer layout still has conflicts, compare its reference-plane and power arrangements with the four-layer PCB stackup options, then state which problem the two added layers should solve.

Additional copper layers can provide more space for signal routing, reference planes, or power distribution. Set priorities based on signal edge rates on critical nets, power needs, and component density, then compare 6-layer PCB stackup options.

Three six-layer PCB stackup examples compared

The three example six-layer stackups below assign three, four, or two copper layers to signal routing. Filter them by the number of signal layers needed, reference-plane locations, and copper area for power. Then check the reference path for each critical signal. The board’s nets and routing needs determine whether a layer order is suitable. For an eight-layer comparison, read the 8-layer PCB stackup guide.

Read the layer order from L1 through L6, top to bottom. S means signal, G means ground reference, and P means power. The selected stackup determines layer assignments and the number of available signal layers. Check component placement, via connections, and routing space to confirm that the layout fits.

The four-signal-layer option keeps both L3 and L4 for signals. Check the spacing between them, nearby traces, and return connections to assess interlayer coupling against the board’s signal requirements. For the two-power-layer option, first confirm the power assignments on L3 and L4. Then check whether the reference planes for the outer signal layers are continuous.

Table 1. Three six-layer PCB layer assignments.

Layer orderAvailable signal layersDesign needChecks before selecting
S/G/P/S/G/SL1, L4, L6Three signal-routing layers, with one copper layer reserved for powerCheck the L2 ground plane as the reference for L1 and the L5 ground plane as the reference for L6. L4 lies between the L3 power plane and the L5 ground plane. Check the dielectric spacing on both sides and copper continuity to determine the applicable reference path for L4.
S/G/S/S/G/SL1, L3, L4, L6More signal-routing space, with power distributed across signal layers or copper regionsCheck the spacing between L3 and L4 and nearby traces. Check the continuity of reference copper on L2 and L5, and the connections used when signals change layers.
S/G/P/P/G/SL1, L6Consider assigning more inner-layer copper area to power networksConfirm the power assignments on L3 and L4. Check whether L2 and L5 provide reference planes for L1 and L6, respectively, and confirm the available signal-routing space.
Three six-layer PCB layer assignments

Figure 1. Six-layer stackup examples showing the signal, ground-reference, and power assignments for three layer orders from L1 through L6.

Reference paths when dielectric spacing changes

When dielectric spacing changes, review the cross-section again. Check the distance from each signal trace to its reference plane, trace width and spacing, and continuity of the reference copper. Mark the relationship between each signal layer and its adjacent reference plane on the six-layer stackup drawing.

Spacing between signal and reference layers from L2 through L5

Figure 2. In the diagram, h_top and h_bottom are the reference spacings from L3 to L2 and L4 to L5, respectively. d_signal is the spacing between L3 and L4. Record layer function and each spacing separately. The drawing is not to scale.

Dielectric separates adjacent copper layers. An outer-layer trace and the nearby reference plane form a microstrip structure. An inner-layer trace between reference planes is usually evaluated as a stripline. Because dielectric thickness changes the geometry between a signal trace and reference copper, results from a previous controlled-impedance analysis cannot be carried over without review.

After setting the layer order, check the signal’s return path to its source. TI explains that, as frequency rises, return current follows a lower-impedance path close to the signal trace. A gap in the reference plane can force that path to detour and increase loop area.

When a signal changes layers, check that a low-impedance connection can link the reference layers before and after the transition. If both reference layers are ground, consider placing ground stitching vias near the signal via. If the signal changes from a ground reference to a power reference, also review the power network and decoupling path.

One six-layer project: materials, lamination, and finished thickness

Record the finished-board thickness requirement separately from the thickness requirements at each lamination stage. Then list the core and prepreg labels. One anonymized six-layer HDI project record specifies FR-4 KB-6165, a finished board thickness requirement of 0.60±0.10 mm, one core listed as 0.17 mm including copper, and four PP1080 prepreg plies labeled 0.075 mm each.

Green PCB panel showing traces and holes

Figure 3. Photograph of a green PCB panel.

The core, prepreg, and copper foil make up the stackup, and lamination bonds them into a board. Count board layers as copper layers. Prepreg (PP) is an insulating dielectric and does not count as a copper layer. Copper cladding on the core and foil added during lamination form the corresponding copper layers. Do not add the PP1080 label thicknesses to derive post-lamination dielectric thickness or finished board thickness.

Table 2. Thickness requirements at each stage of the project.

StageThickness requirementHow to read it
Project first lamination0.35±0.05 mmThickness requirement for the first lamination stage listed on the process card
Project second lamination0.50±0.05 mmThickness requirement for the second lamination stage listed on the process card
Project finished board0.60±0.10 mmFinished board thickness requirement listed in the product specification and final inspection record

Six-layer PCB fabrication: five checks before production

Complete the DFM review before fabrication, covering copper-layer files, via structure, material dimensions, impedance requirements, and revision control. For the full layer order and material relationships, see the multi-layer PCB stackup guide. When preparing a package for bare-board PCB manufacturing, match the finished board thickness and tolerance, material combination, via connection range, and impedance requirements to the same revision of the engineering files. Include the quantity and any routing conditions that need confirmation when requesting a bare-board manufacturing quote.

  1. Map the copper-layer files. Confirm that the six Gerber copper layers map to L1 through L6, and list each layer’s signal, ground-reference, or power role in the stackup table.
  2. Specify via types and connection ranges. Distinguish plated from non-plated holes. For blind or buried vias, list the start and end layers for each via group and match them to the drill files.
  3. List material and thickness requirements. Name the core, prepreg, copper foil, finished copper thickness, finished board thickness, and tolerances, with units. Record material labels separately from post-lamination and finished-board requirements.
  4. List controlled-impedance requirements. State whether each net is single-ended or differential, its target impedance and tolerance, signal layer, reference layer, trace width, and spacing. Note which dimensions can change. Record target values as fabrication-review requirements, not as measurement results.
  5. Check revision and approval status. Use the same revision number for layer files, drill files, the stackup table, the mechanical drawing, and fabrication notes. Record changes that need confirmation from the fabricator. After review, submit the bare-board quote with this version of the file package.

Table of Contents

You Might Also Like