PCB EditorIPC-2141

Stackup and controlled impedance in Allegro X: from Cross-section to the fab

How to build the layer stackup, calculate impedance in the cross-section editor and align everything with your fabricator.

8 min read

Why the stackup comes first

The layer stackup defines trace impedance, coupling between signals, the quality of return planes and even whether the board will warp in the reflow oven. Changing it after routing means redoing widths and spacings. Define it at the very beginning — ideally starting from your fabricator's standard stackup.

Mask L1 TOP — signal (microstrip) Prepreg L2 GND — reference plane Core L3 SIG — stripline Prepreg L4 SIG — stripline Core L5 PWR/GND — plane Prepreg L6 BOTTOM — signal (microstrip) Mask
Example 6-layer stackup: outer signals as microstrip, inner signals as stripline between planes.

The cross-section editor

In Setup > Cross-section you define, for each layer:

  • Type: conductor (signal), plane or dielectric (core/prepreg).
  • Material and thickness: copper (e.g., 1 oz ≈ 35 µm) and dielectric with dielectric constant (Dk) and loss factor (Df).
  • Trace width and pair spacing: Allegro computes single-ended and differential impedance with a field solver, and can also work backwards (target impedance → width).

Tip: create a board template with the approved stackup and matching rules. New designs start out right.

Stackup good practices

  • Symmetry around the center (thicknesses and copper distribution) to reduce warpage. IPC-6012 limits bow & twist; for boards with SMT parts the usual limit is 0.75%.
  • Every high-speed signal layer next to a solid plane, for the current return path.
  • Avoid two adjacent signal layers without a plane between them; if unavoidable, route them orthogonally.
  • Closely spaced power and ground planes increase distributed capacitance and help decoupling.

Alignment with the fabricator

The value computed in software is an estimate. The fabricator adjusts width and dielectric to the real materials and delivers an impedance test coupon. In the fab notes, state: target impedance per layer and width, tolerance (typically ±10%), materials (per IPC-4101) and the sentence “the fabricator may adjust widths to meet impedance”.

Note: Dk varies with frequency and with the glass/resin system. Use the material value at the frequency of interest, not the generic “FR-4 = 4.5”.

Related standards

  • IPC-2141 — design guide for high-speed controlled-impedance circuit boards.
  • IPC-2221 / IPC-2222 — generic and rigid-board design requirements.
  • IPC-4101 — base materials specification (laminates and prepregs).

References and further reading

Original text for educational purposes. Menus and commands may vary between Allegro X versions; check the Cadence documentation for your version.