PCB impedance calculator

A signal on a trace travels as a wave between the trace and its return path, a plane below or above it or the copper beside it. The ratio of its voltage to its current is the characteristic impedance Z0, which a trace must match to its driver and receiver for the signal to arrive without reflections. It depends on the width of the trace, its distance from the planes and the permittivity of the dielectrics around it. Closed-form formulas, such as those of Hammerstad and Jensen for the microstrip, give it for a few simple cross-sections. The tool solves the electric field of the actual cross-section with the finite element method, with the trace's thickness and etched flanks, the solder mask, several dielectrics and the copper beside the trace.

The stackup

The stackup table lists the board's layers from top to bottom, as the board house specifies them: solder mask, copper and dielectric, each with its thickness t. A dielectric layer, a core or a prepreg, has a material with its relative permittivity εr and its loss tangent tan δ. The list fills in typical values, which should be replaced by those of the laminate's data sheet at the frequency of interest. A copper layer has a role:

• Trace is the layer of the trace or the pair, and two layers have it for a broadside-coupled pair.
• Plane is a reference plane, ground or power, that runs under the whole trace.
• Unused is copper that the trace does not see, filled with the dielectric around it.

The planes nearest to the trace bound its field, and the layers beyond them do not matter. A trace with a plane on one side only is a microstrip on an outer layer, or an embedded microstrip under further dielectric. A trace between two planes is a stripline, centered or offset. The Board list fills the table with a common stackup of 2, 4 or 6 layers and 1.6 mm, + Layer pair adds a dielectric and a copper layer above the bottom one, and Open a KiCad board reads the stackup of a .kicad_pcb file.

Traces and pairs

The trace is a single trace, an edge-coupled pair side by side on one layer, or a broadside-coupled pair on two layers, one trace above the other. Its width w is the width at its base, where it sits on the dielectric, and the spacing s of an edge-coupled pair is the gap between its two traces at the base. The copper's thickness comes from the trace's layer, and a thickness of 0 gives an infinitely thin trace, as the closed-form formulas assume. With Coplanar ground on, copper at 0 V lies beside the trace or the pair on the same layer, at the gap g, and reaches out sideways without end, as a ground pour does. A microstrip with a coplanar ground is a grounded coplanar waveguide.

Solder mask and etching

A solder mask layer covers the outer copper and the dielectric between it with a coat of the layer's thickness, which follows the flanks of the trace. Since the mask puts dielectric where there was air, it lowers the impedance of an outer trace. An etched trace is narrower at its top than at its base. With an etch angle α below 90° its flanks lean in, and its top is w − 2t/tan α wide, which raises the impedance a little.

Results

For a single trace the results give its impedance Z0 and its effective permittivity εeff, the permittivity of a uniform medium in which the signal would travel as fast as on the trace. They also give the delay per length, √εeff/c, and the inductance and the capacitance per length. For a pair they give the differential impedance Zdiff between the two traces, the common-mode impedance Zcommon of both traces driven together against the planes, and the odd-mode and even-mode impedances of each trace, Zodd = Zdiff/2 and Zeven = 2·Zcommon, with the effective permittivity and the delay of both modes. For a pair whose two traces are not alike, such as a broadside pair between unequal dielectrics, these come from the impedance matrix of the two lines. The drawing colors the cross-section by the potential or the field strength, with the trace at 1 V, and a pair driven with +1 V and −1 V in the odd mode or with +1 V on both in the even mode.

Losses

With Losses on, the results add the attenuation at the frequency given, in dB per meter, or per inch when the lengths are in mils, in two parts:

• The dielectric loss comes from each dielectric's tan δ, weighted by the share of the electric field's energy in it.
• The conductor loss comes from the copper's conductivity. The current flows in a layer about a skin depth thick at the surface of the trace and of the planes, and the tool integrates its losses over every copper surface. This holds once the skin depth is small against the copper's thickness, from about 100 MHz for 35 µm copper.

The copper counts as smooth. The roughness of real copper raises the conductor loss at high frequencies and is not part of the results.

Target impedance and width sweep

With a Target, the tool searches for the trace width that gives it, Z0 for a single trace and Zdiff for a pair at the given spacing. A secant search solves the cross-section again for each width it tries and stops within 0.01 % of the target, and the results show the width with the impedance it reaches. Leave Target empty to skip the search. The width sweep solves the cross-section for a range of widths and shows the impedance over the width as a table and a chart.

KiCad boards

Open a KiCad board reads the stackup that KiCad's Board Setup saves in a .kicad_pcb file: the solder masks, the copper layers and the dielectrics with their thickness, material, εr and loss tangent, including dielectrics made of several sublayers. The first copper layer becomes the trace's layer and the second a plane, which you can change in the table. A board whose stackup was never set up in KiCad has none in its file, and the table then stays as it is. The tool reads only the stackup, not the tracks.

Units

Lengths are in millimeters or mils, as the Unit list sets them, and a change of the unit converts the table and the trace. The frequency is in GHz, the conductivity in MS/m, the delay in ps and the inductance and the capacitance per millimeter, or per inch for mils. The drawing is in millimeters, with the potential in volts and the field strength in V/mm.

1. Load

   The page loads Python and planex2d into this tab, and NGSolve with the first solve, about 23 MB the first time. Your browser keeps them in its cache, so later visits start faster.

2. Draw

   planex2d draws the cross-section from the stackup and the trace, with the copper as exact polygons and the solder mask as an offset of the copper.

3. Solve

   NGSolve meshes the cross-section and solves its electric field with the dielectrics and in air, again whenever a setting changes after the first solve.

4. Save

   The results are saved as a PDF report or a CSV table, and the cross-section as a DXF file, made in the tab as well.

The finite element model

The unknown is the electric potential in the cross-section. The copper is a perfect conductor, with the traces at their voltages and the planes and the coplanar ground at 0 V. The board's layers run on sideways without end, and an open side above or below the board reaches to infinity. The tool models this with zones at the sides of the cross-section that a coordinate map stretches out to infinity along x, and zones above and below it stretched along y. The layers keep their thickness all the way out, and the result does not depend on the size of a box. For each trace, one solution with the dielectrics and one with air everywhere give the capacitance matrices C and C0 per length, the inductance matrix L = μ0ε0·C0⁻¹, and from them the impedances and the delays. The mesh is refined geometrically toward the corners of the copper, where the field is singular, 3 levels deep by default, and NGSolve solves with fourth-order elements and a sparse Cholesky factorization. Both are set in the Solver group.

How it is tested

The tests solve cross-sections whose impedance is known exactly, with infinitely thin traces as the formulas assume, and compare the tool's values with those, at its default settings. Hammerstad and Jensen's formulas are fits, which they state to hold within 0.01 % for the impedance of a microstrip in air and within 0.2 % for the effective permittivity on a substrate. The conductor loss is compared with Wheeler's incremental inductance rule, which gives the same loss from the change of the inductance when every copper surface recedes by a small step.

Supported files

Run it in Python

The same analysis takes a few lines with planex2d and NGSolve. The example is a centered stripline, an infinitely thin strip of 0.5 mm halfway between two planes 1 mm apart, in a dielectric of εr 4. planex2d draws the space between the planes as two faces with the strip on their common edge, and NGSolve solves for the potential with the strip at 1 V and the planes and the far ends at 0 V. In a single dielectric the field energy gives the impedance directly, Z0 = √εr/(c·C) with C = ε∫|∇V|². See Meshing with netgen in the docs, and the microstrip impedance example for a microstrip and the width for 50 Ω.

$ pip install "planex2d[occ]" ngsolve

import math

import ngsolve as ngs
import planex as px

b, w, er = 1.0, 0.5, 4.0
lower = px.QuickSketch((-5, 0)).Rectangle(10, b / 2).Face()
upper = px.QuickSketch((-5, b / 2)).Rectangle(10, b / 2).Face()
strip = px.Line((-w / 2, b / 2), (w / 2, b / 2))
board = px.Glue([lower, upper, strip])
for e in board.edges:
    m = e.midpoint
    if strip.Distance((m.x, m.y)) < 1e-9:
        e.name, e.maxh = "strip", 0.01
    elif abs(m.y) < 1e-9 or abs(m.y - b) < 1e-9 or abs(abs(m.x) - 5) < 1e-9:
        e.name = "ground"
mesh = ngs.Mesh(px.OCCGeometry(board).GenerateMesh(maxh=0.2))
fes = ngs.H1(mesh, order=4, dirichlet="strip|ground")
u, v = fes.TnT()
a = ngs.BilinearForm(ngs.grad(u) * ngs.grad(v) * ngs.dx).Assemble()
V = ngs.GridFunction(fes)
V.Set(1, definedon=mesh.Boundaries("strip"))
r = V.vec.CreateVector()
r.data = -a.mat * V.vec
V.vec.data += a.mat.Inverse(fes.FreeDofs(), inverse="sparsecholesky") * r
energy = ngs.Integrate(ngs.grad(V) * ngs.grad(V), mesh)
eta0 = 4e-7 * math.pi * 299792458
Z0 = eta0 / (math.sqrt(er) * energy)


def K(k):
    x, y = 1.0, math.sqrt(1 - k * k)
    for _ in range(8):
        x, y = (x + y) / 2, math.sqrt(x * y)
    return math.pi / (2 * x)


k = 1 / math.cosh(math.pi * w / (2 * b))
print("Z0", round(Z0, 3), "ohm, exact", round(eta0 / (4 * math.sqrt(er)) * K(k) / K(math.sqrt(1 - k * k)), 3))

It prints an impedance of 50.176 Ω, against 50.216 Ω from Cohn's exact formula. The tool also refines the mesh toward the strip's edges, where the field is singular, and comes within 0.004 %.

Privacy

Limits

• The model is quasi-static, the field of the cross-section at rest, which holds while the cross-section is small against the wavelength. At tens of GHz the impedance and the effective permittivity change with the frequency, which the tool does not compute.
• The trace is straight and long, over planes without gaps. Vias, bends, splits in a plane and the stitching vias of a coplanar ground are not part of the model.
• The copper is smooth, and inside it the field is zero. Its roughness and the current inside it at low frequencies are left out.
• Each material has one εr and one tan δ, the values of its data sheet at the frequency of interest. The glass weave and the resin content of a real laminate vary them.
• A board that fails or a result that looks wrong? Open an issue on GitHub and attach the stackup if you can.