Grounded coplanar waveguide: 50 Ω width, gap and vias
Size a grounded coplanar waveguide for 50 Ω: 0.45 mm trace and 0.25 mm gaps over 0.3 mm of FR-4, 1.25 mm on a 1.6 mm board, via fencing and the model's limits.
A 50 Ω grounded coplanar waveguide on a four-layer FR-4 board is a 0.45 mm trace with a 0.25 mm gap on each side, 0.3 mm above the first inner plane. That is the line Silicon Labs publishes for its 2.4 GHz radio boards, and the closed-form model reads it as 51.9 Ω with 35 µm copper. On a 1.6 mm two-layer board the same gaps need a 1.25 mm trace, where a microstrip needs 2.88 mm. Stitch the side grounds to the plane with vias no more than about 1.25 mm apart at 2.4 GHz. Three inputs set the impedance: the ratio W/(W + 2G), the height H to the plane, and εr. The copper thickness is a correction of a few per cent on top.
Every derived number below comes from the module behind the coplanar waveguide calculator, so the two agree. The equations are those of the Qucs technical documentation, cross-checked against Sandia’s report SAND2017-12410J, which prints two of them wrongly; the layout rules are from Silicon Labs AN928.1 and AN928.2.
What sets the impedance of a grounded coplanar waveguide
A coplanar waveguide is a signal trace with a ground pour on each side of it, on the same layer. Sandia’s report (p. 1) names the PCB variant:
The designs, where the distance of the bottom conductor is close enough to the CPW line to influence the characteristics, is referred as conductor backed CPW or more commonly grounded CPW (CPWG).
GCPW, CPWG and conductor-backed CPW are the same structure. Here W is the trace width, G each gap, H the dielectric height to the plane and T the copper thickness, which are Sandia’s letters; Qucs writes the gap as s.
The field leaves the signal trace three ways: across the gaps through the air, across the gaps inside the laminate, and down to the plane. Conformal mapping turns each region into a parallel-plate capacitor whose capacitance is a ratio of complete elliptic integrals, K(k)/K′(k), with one modulus for the top copper and one for the plane (Qucs Eq 12.10 to 12.13):
The k1 term is the coplanar part and contains only a ratio. Sandia states the consequence for a line with no plane (p. 1): “the characteristic impedance of the CPW is not a function of the transmission dimensions, instead a function of the ratio of the dimensions.” The k3 term is what the plane adds, and it brings H in. Qucs describes the result in one sentence: “In this case, the quasi-TEM wave is an hybrid between microstrip and true CPW mode.” The filling factor q is the share of the line’s air-equivalent capacitance that sits below the copper, in the dielectric. It is exactly 0.5 for a coplanar line on an infinitely thick substrate and 0.62 for the Silicon Labs line.
Sandia’s rule for when the plane can be ignored is Eq 36 (p. 11), H ≫ 2(W + 2G). For a 0.45 mm trace with 0.25 mm gaps that is H ≫ 1.9 mm. No standard board meets it, so a coplanar line on a PCB with copper underneath is a grounded one and has to be calculated as one. The same trace and gaps on 0.3 mm of laminate with nothing below would be 71.0 Ω; with the plane they are 51.9 Ω.
Worked example: the 0.45 mm trace with 0.25 mm gaps
AN928.2 Table 3.1 (p. 28) gives the “Parameters for 50 Ω Grounded Coplanar Lines” of the four-layer BRD4180A radio board: f 2.4 GHz, T 0.018–0.035 mm, εr 4.6, H 0.3 mm, G 0.25 mm, W 0.45 mm. Its first note defines H:
For PCBs with more than 2 layers, ‘H’ is the distance between the top and the first inner layer. For 2-layer PCBs, ‘H’ is the distance between the top and the bottom layer.
Through the equations above, then the thickness correction described further down:
k1 0.45 / 0.95 = 0.4737 k3 tanh(π·0.45/1.2) / tanh(π·0.95/1.2) = 0.8384 q filling factor = 0.6156 ε_re 1 + 0.6156 × (4.6 − 1) = 3.216 Z, T = 0 = 53.3 Ω Z, T = 18 µm = 52.5 Ω Z, T = 35 µm ε_re falls to 2.963 = 51.9 Ω
The model does not land on 50 Ω, and the difference is left in view. Two things are known about it. The model is for bare copper, and solder mask over a line adds capacitance, which lowers the impedance. And the two Silicon Labs notes disagree with each other: AN928.1 Table 2.1 (p. 10) lists the same W and G as a 50 Ω line on H = 0.325 mm, which the model reads as 53.5 Ω. Both tables cannot be exactly 50 Ω with one geometry on two heights. The notes allow for it: “Different impedance calculators may yield slightly different results.” To put the model exactly on 50 Ω at H = 0.3 mm, the gap would close to 0.20 mm or the trace widen to 0.48 mm.
At 2.4 GHz the wavelength on this line is 72.6 mm and the delay 5.74 ps/mm.
Trace width for 50 Ω on common stackups
The table gives the width for 50 Ω at three gaps, for the dielectric heights that standard stackups put under the top layer, at εr 4.6 with 35 µm copper. The last column is the microstrip width on the same height from the IPC-2141 closed form in the microstrip impedance calculator. On a multilayer board H is the prepreg between the top layer and the first inner plane, which the PCB stackup article explains should be a solid ground.
| H to the plane | G = 0.15 mm | G = 0.25 mm | G = 0.5 mm | Microstrip |
|---|---|---|---|---|
| 0.1 mm | 0.17 mm | 0.19 mm | 0.20 mm | 0.14 mm |
| 0.2 mm | 0.30 mm | 0.35 mm | 0.38 mm | 0.32 mm |
| 0.3 mm | 0.39 mm | 0.48 mm | 0.55 mm | 0.50 mm |
| 0.36 mm | 0.44 mm | 0.55 mm | 0.65 mm | 0.61 mm |
| 0.8 mm | 0.63 mm | 0.92 mm | 1.23 mm | 1.42 mm |
| 1.0 mm | 0.67 mm | 1.03 mm | 1.44 mm | 1.78 mm |
| 1.6 mm | 0.73 mm | 1.25 mm | 1.93 mm | 2.88 mm |
Read along the top rows and the plane dominates: at H = 0.1 mm the width moves only from 0.17 to 0.20 mm across the whole range of gaps. Read along the bottom row and the side grounds do the work. AN928.2 warns about copying its table across (p. 28): “A 2-layer PCB requires different parameters for a 50 Ω transmission line than shown in this table due to the different value of “H”.” The model agrees. The 0.45 mm trace with 0.25 mm gaps is 69.5 Ω on a 1.6 mm board.
The top rows need a caution. At H = 0.1 mm the microstrip column is narrower than every coplanar one, and down to 0.36 mm it is still narrower than the G = 0.5 mm column. That cannot be physical, because side grounds only add capacitance, so a coplanar trace is always the narrower of the two. It is two closed forms disagreeing where 35 µm of copper is a large fraction of the dielectric: the IPC-2141 fit is a curve fit and the coplanar result is a conformal map with a first-order thickness correction. On dielectrics that thin, use the fabricator’s field solver.
How much the gap changes the impedance
AN928.2 (p. 28) says of the gap:
Characteristic impedance is not “super sensitive” to the gap value. It should be between 0.25 and 0.4 mm to have 47 through 53 Ω impedance.
Run through the model at W = 0.45 mm, H = 0.3 mm and 35 µm copper, the gap does this:
| G | 0.15 mm | 0.25 mm | 0.4 mm | 1 mm | 2 mm |
|---|---|---|---|---|---|
| Z₀ | 46.8 Ω | 51.9 Ω | 55.0 Ω | 58.7 Ω | 60.7 Ω |
From 0.25 to 0.4 mm the model moves 3.1 Ω, half the 6 Ω span the note quotes and offset upward by about 5 Ω, so it agrees on the weak dependence and not on the absolute figure. With the plane only 0.3 mm down, field that no longer crosses a wider gap goes to the plane instead. Past 1 mm the side grounds hardly matter and the line is nearly a microstrip. The steep end is below 0.2 mm, where each 0.05 mm is worth about 2 Ω.
The etch tolerances compare as follows on the same line. A trace 0.05 mm wide or narrow gives 49.1 or 55.1 Ω. A gap 0.05 mm narrow or wide gives 49.9 or 53.2 Ω. εr of 4.2 or 4.8 gives 53.9 or 51.0 Ω. Width is the strongest lever, and since over-etching narrows the trace and widens both gaps together, the two errors add.
GCPW vs microstrip: which to choose
Silicon Labs gives its reason for the coplanar line in AN928.2 (p. 27):
To reduce sensitivity to PCB thickness variations, use 50 Ω grounded coplanar lines where possible for connecting the antenna or the U.FL connector to the matching network. This also reduces radiation and coupling effects.
The first claim can be checked with the model. Take a 50 Ω line, change H by 1 % and see how far the impedance moves.
The IPC-2141 microstrip moves 0.71 % per per cent of H at 50 Ω, whatever the stackup, because its impedance is a logarithm of H. The Silicon Labs line moves 0.41 %. A dielectric 10 % thin or thick takes the microstrip to 46.3 or 53.4 Ω and the coplanar line to 47.8 or 51.9 Ω. The claim holds, and it is a modest gain at H = 0.3 mm. On a 1.6 mm board with 0.25 mm gaps the figure is 0.11 %: the same ±10 % moves the line only between 49.4 and 50.5 Ω. The benefit grows as the gap shrinks relative to the height, and disappears as the gap widens.
The second reason is width. Sandia makes the point for thick substrates (p. 8): a microstrip there needs “a wider top conductor”, so that “a microstrip line for a thick substrate is often become impractical”. On a 1.6 mm board that is 2.88 mm of trace against 1.25 mm, feeding parts whose pads are a fraction of a millimetre wide.
The third is the return path. Shunt matching parts, ESD diodes and connector grounds land on a ground that is on the same layer, a gap away.
Microstrip is the better choice when the dielectric is thin and the route is long. At H = 0.2 mm or less the plane carries most of the field either way (the width column barely changes with the gap), and the side grounds add copper features to etch and vias to drill for little return. It is also the choice when the top layer cannot give each side a ground at least as wide as the rule below, because a narrow unstitched sliver is worse than no side ground.
Whether a trace needs a controlled impedance at all is a length question. AN928.2’s threshold (p. 27) is “to use 50 Ω transmission lines where the length of the RF trace is longer than λ/16 at the fundamental frequency”, and λ/16 on this line at 2.4 GHz is 4.5 mm. Shorter interconnects between matching components are, in the note’s words, “not considered transmission lines”. For digital edges the critical length calculator applies the equivalent test against rise time.
Via fencing: how close the stitching vias need to be
The formulas assume the two coplanar grounds and the plane are one conductor. Vias make that true. AN928.2’s instruction for the line itself (p. 27) is “Use many vias near the coplanar lines in order to minimize radiation”, and the spacing comes from its general rule (p. 19):
Use a series of GND stitching vias along the PCB edges and internal GND metal pouring edges. The maximum distance between the vias should be less than lambda/10 of the 10th harmonic (the typical distance between vias on reference radio boards is 40–50 mil).
The note does not say which wavelength. At 2.4 GHz the 10th harmonic is 24 GHz, and λ/10 there is 1.25 mm in free space or 0.73 mm at this line’s εeff of 2.96. The quoted 40–50 mil is 1.02–1.27 mm, so the free-space wavelength is the reading that matches the note’s own boards.
Sandia’s figure is far looser. Writing about chips, where the grounds are joined by air-bridges across the signal, it says (p. 9): “This ground connection needs to be repeated at least at every quarter wavelength of the highest operating frequency.” A quarter wave at 2.4 GHz on this line is 18.1 mm. The two rules protect different things. Sandia’s keeps the two slots balanced at the operating frequency so that the slot-line mode it describes is not excited. Silicon Labs’ is set by harmonic radiation from the pour edges, at ten times the frequency. A radio that has to pass a spurious emission test needs the tighter one.
None of the three sources gives the distance from the gap to the via row, and the closed-form model has no term for the vias at all.
Ground width and spacing between two lines
The model assumes the side grounds extend forever. Sandia gives two rules of thumb for real ones (p. 10). Eq 34 sets the width WG of each ground, and Eq 35 the ground d between two lines for “sufficient (> 30dB) isolation”:
The first rearranges to WG > (W + 2G)/2. For the Silicon Labs line that is 0.475 mm of copper beside each gap, and 1.9 mm of ground between two such lines. A pour that necks down to less than that beside a connector pin or under a shield wall is not the ground the 50 Ω figure assumed.
Copper thickness and solder mask
Qucs gives a first-order correction for the copper (Eq 12.14 to 12.18, from Gupta et al.). The edges of the trace and grounds move toward each other by Δ, and the air between the side walls lowers εre:
For 35 µm on the worked line Δ is 0.085 mm, a third of the gap, and the result is 51.9 Ω against 53.3 Ω for zero thickness, a 2.6 % correction. Qucs presents the correction for the coplanar line in general. Applying it to the grounded line with k3 left unchanged is the calculator’s reading, not something either source states, and the calculator flags it once T exceeds a fifth of G or W.
Solder mask is outside the model entirely. It replaces air in and above the gaps with dielectric, which can only lower the impedance, and none of the three sources puts a number on it for a coplanar line. Either open the mask over the line or have the fabricator include it.
Where the closed-form model stops
The model is quasi-static: Z₀ and εeff do not depend on frequency. Qucs gives the frequency scale at which that fails, the cut-off of the substrate’s TE₀ surface mode (Eq 12.24):
For εr 4.6 that is 131.7 GHz at H = 0.3 mm and 24.7 GHz at H = 1.6 mm. The 10th harmonic of 2.4 GHz sits at the cut-off of a 1.6 mm board, which is one more reason the via rule is written around it. Qucs’ dispersion expression (Eq 12.19 to 12.23, “claimed to be better than 5%” inside its stated ranges) raises εeff of the worked line by 0.03 % at 2.4 GHz. For the 1.25 mm line on a 1.6 mm board it gives 0.15 % at 2.4 GHz, 0.8 % at 6 GHz and 1.9 % at 10 GHz. Qucs writes that expression for the coplanar line generally, so on a grounded line treat those as an indication of scale.
The geometry has limits too. Sandia says of its own analysis (p. 2):
In addition, the effect of the finite ground plane and the metal thickness has not been considered in the analyses presented.
Not modelled anywhere here: finite ground width, the via fence, solder mask, unequal gaps, a trapezoidal etch profile, a second dielectric, conductor and dielectric loss, and the other modes a three-conductor line supports. Sandia lists those (p. 8): slot-line modes between the grounds, a microstrip mode to the plane, and parallel-plate modes between top copper and plane. It also writes that “the presence of a ground plane might introduce other non-CPW modes and interfere with the CPW operation”, which reads as advice against the grounded line that Silicon Labs recommends. The two are reconciled by the vias: Sandia is describing chips where, in its words, an “extra ground via process is unnecessary”, and a PCB line is only well behaved because the fence shorts those modes out.
For anything the list above touches, Sandia’s own recommendation (p. 9) is “3-dimensional simulators based on Fine Element Method (FEM)”. In practice that means ordering controlled impedance and letting the fabricator set the final width for its stackup and mask.
Two misprints in the Sandia report
The Sandia report is the more readable source and two of its equations do not work as printed. Both were checked by running them.
Eq 18 (p. 5), the impedance of the conductor-backed line, is printed with a denominator of K′(k)/K(k) · K(kG)/K′(kG) alone. For the worked line at zero thickness that gives 65.6 Ω where Qucs Eq 12.13 gives 53.3 Ω. With the “1 +” of the report’s own Eq 17 restored and a factor K′(k)/K(k) in front, it becomes Eq 12.13. Eq 17, the effective permittivity, is correct as printed and returns the same 3.216.
Eq 12 (p. 4), Hilberg’s approximation for k ≤ 1/√2, is printed with √k where Qucs Eq 12.4 has √k′. At k = 0.4737 the printed form returns 1.319 for K(k)/K′(k); the exact value is 0.758, which Qucs’ form reproduces to four places. The report also numbers two different equations (19) on the same page.
A procedure for a 50 Ω grounded coplanar line
- Take H from the stackup: top layer to the first plane, not the board thickness, unless the board has two layers.
- Choose the gap. The fabricator’s minimum spacing is the floor; a gap somewhat wider costs little impedance and varies less in proportion.
- Solve for W with the calculator at the laminate’s εr and the finished copper thickness.
- Give each side ground at least (W + 2G)/2 of unbroken copper and a row of vias at λ/10 of the 10th harmonic or closer.
- Keep the plane under the line and both grounds solid.
- Hand the fabricator the target impedance, and treat the calculated width as the starting point.
Sources
- Qucs technical documentation, Coplanar waveguides (CPW). Eq 12.4 to 12.5, Hilberg’s K/K′ approximation; Eq 12.6 to 12.13, the coplanar line on an infinite, finite and conductor-backed substrate; Eq 12.14 to 12.18, the metal thickness correction; Eq 12.19 to 12.24, dispersion and the TE₀ cut-off.
- Shahed Reza, Coplanar Waveguide and Applications, SAND2017-12410J, Sandia National Laboratories. Definition of the grounded line and the ratio property (p. 1); assumptions (p. 2); Eq 12 (p. 4); Eq 17 to 19 (p. 5); advantages, the thick-substrate comparison with microstrip and the non-CPW modes (p. 8); thickness, field simulators and the quarter-wave ground connection (p. 9); Eq 34 and 35 (p. 10); Eq 36 (p. 11).
- Silicon Labs, AN928.2: EFR32 Series 2 Layout Design Guide, Rev. 1.7. Stitching via spacing (p. 19); the reasons for grounded coplanar lines, the λ/16 rule and vias near the line (p. 27); Table 3.1 and its notes (p. 28).
- Silicon Labs, AN928.1: EFR32 Series 1 Layout Design Guide, Rev. 0.6. Table 2.1, the same line on H = 0.325 mm (p. 10).