A solid copper ground plane is the best electrical reference and the worst thing to put in a bend. A hatched (cross-hatch) plane is the standard compromise: a grid of copper lines that keeps a return path and some shielding while letting the layer flex with much less stress. But a hatch is not "a solid plane with holes." Its line width, pitch and angle change the copper fill, the impedance under your traces and the path return current takes. Get them wrong and a board that passed on solid copper drifts out of impedance the moment you hatch it.
This guide covers the geometry math you can check yourself, what hatching does to impedance and return current, where a hatch belongs (and where it does not), and how to write the drawing so the fab house builds the pattern you designed.
Judgment first: when to hatch, when to stay solid
Use the plane where its job is:
- Solid plane where the board is static, and always under controlled-impedance or high-speed pairs you need to model tightly — including the rigid sections of a rigid-flex.
- Hatched plane in the flexing region, where solid copper is the stiffest and most crack-prone layer in the stack-up.
- Shielding film or silver ink instead of a plane when the bend is truly dynamic and you need shielding but cannot afford copper in the bend — see our EMI shielding materials guide for the comparison.
If the answer is "solid where static, hatched (or film) only where it bends," you usually get most of the electrical benefit and most of the flexibility. Hatching the whole board "to be safe" gives up controlled impedance everywhere for a benefit that only exists in the bend.
The hatch geometry, with the math
A hatch is defined by two numbers: line width (w) and pitch (p), the centre-to-centre spacing of the lines. For an orthogonal grid the openings are squares of side (p − w), and the copper fill is:
fill = 1 − ((p − w) / p)²
That is arithmetic, not a vendor claim, so you can check any pattern in seconds:
| Line width w | Pitch p | Opening side (p − w) | Copper fill |
|---|---|---|---|
| 0.10 mm | 0.50 mm | 0.40 mm | 36% |
| 0.15 mm | 0.50 mm | 0.35 mm | 51% |
| 0.25 mm | 0.50 mm | 0.25 mm | 75% |
| 0.15 mm | 0.30 mm | 0.15 mm | 75% |
| 0.10 mm | 0.30 mm | 0.20 mm | 56% |
Two things follow. Fill is the lever for flexibility — less copper is a more compliant layer — while opening size is the lever for electrical behaviour. The same 75% fill can be built as fine lines at a tight pitch or wide lines at a coarse pitch, and the fine version has openings less than half the size. For a given fill, prefer the finer pitch your fabricator can etch reliably, because small openings disturb the return path less.
The lines must also be etchable: very narrow lines at high fill are a yield risk on thin copper, so agree the minimum line and space with the supplier before you commit — the copper thickness guide covers how foil weight limits fine features.
What hatching does to impedance
Impedance depends on the capacitance between the trace and its reference. A hatched plane removes copper under the trace, so that capacitance falls and the characteristic impedance rises compared with the same stack-up on a solid plane. How much depends on the fill, the trace width, the dielectric thickness and whether the trace sits over a line or an opening. There is no honest single number — model your actual geometry in a field solver, then verify with an impedance coupon (see impedance coupons: design and test).
The geometry gives you one hard rule. A trace narrower than the opening can sit entirely over a hole. With the 0.15 mm / 0.50 mm hatch above, the openings are 0.35 mm wide, and a 0.10 mm flex trace can run straight down the middle of one with no copper beneath it for a long stretch — and then cross a line and jump back. That periodic swing in impedance is what people mean when they say a hatch "ruins" a controlled-impedance line.
Keeping the return path honest
Return current wants to flow directly under the signal. Over a hatch it has to detour around openings, which lengthens the loop and raises inductance; the coarser the hatch relative to the trace, the bigger the detour. Practical rules:
- Route at an angle to the hatch. Running the hatch at 45° to the trace direction means the trace crosses lines continuously instead of tracking along an opening or along a line. The alternative — a trace parallel to a hatch line — gives the worst case: either always over copper or always over a gap, and a step where it changes.
- Keep openings small relative to trace width and spacing. If a pair's spacing or a trace's width is smaller than an opening, the field sees the hatch as a series of individual windows, not a plane.
- Stagger the hatches on the two reference layers. In a stripline-style stack-up with planes above and below, offset the two hatches by half a pitch so the openings do not line up into a see-through window.
- Do not split or step the hatch under critical signals. Keep the pattern uniform under the whole run of a controlled-impedance pair, and change to solid only at defined transitions.
A note on shielding, because it is often over-worried. The aperture leakage rule of thumb is to keep openings well below about one-twentieth of a wavelength. Free-space λ/20 is about 15 mm at 1 GHz, 3 mm at 5 GHz and 1.5 mm at 10 GHz, so a 0.35 mm opening is far below it in that range — the aperture itself is rarely the limit on a fine hatch. What degrades is the return path and impedance stability, not simple slot leakage. A coarse hatch with multi-millimetre openings is where the aperture rule starts to bite.
Hatching for bend life
The reason to hatch is mechanical, so design it for the bend:
- Angle the lines at about 45° to the bend axis so no long copper line runs parallel to the fold and concentrates strain along one edge. This is common flex practice; confirm the direction against your fabricator's guidance and the bend radius design guide.
- Use rolled annealed copper in the flexing region — hatching softens the layer, but the grain of the foil still sets fatigue life. See RA vs ED copper.
- Avoid stitching vias and heavy copper features inside the bend; put them where the board is static, and follow the wider dynamic bend life design guide.
- Solid-to-hatch transition: move from solid to hatched copper with a gradual change outside the tightest part of the bend, not as an abrupt edge at the bend line.
Also remember that adhesive-based constructions flow into the openings during lamination. The dielectric in the hole is not air, and its thickness feeds into impedance — one more reason to model the finished stack-up rather than the drawing alone, as covered in the multilayer flex stack-up guide.
How to specify it on the drawing
Do not just write "hatched ground." Give the fab house:
- Line width, pitch and angle as numbers, plus the intended copper fill.
- The exact region the hatch covers, with the solid-to-hatch boundary dimensioned.
- The impedance requirement and reference layer, so the supplier can compare the hatched build against the target and propose a stack-up.
- A coupon requirement if impedance matters, built with the same hatch as the real board, not with a solid reference.
Our flex PCB impedance control service reviews the reference-plane design against your target before release, and the flex PCB service page lists what to include in the package.
FAQ
What hatch pattern should I use for a flex PCB ground plane?
Start from the electrical need, then set the numbers: an orthogonal or 45° grid, the finest pitch your fabricator can etch reliably, and a line width that gives the copper fill you need (fill = 1 − ((p − w)/p)²). A finer pitch at the same fill gives smaller openings and a steadier return path. Confirm the pattern with your supplier's minimum line/space and verify impedance on a coupon.
Does a hatched ground plane change impedance?
Yes. Removing copper under the trace lowers the trace-to-plane capacitance, so characteristic impedance rises versus a solid plane in the same stack-up, and it can vary along the trace as it crosses lines and openings. Model the real hatch in a field solver and verify with a coupon rather than reusing solid-plane numbers.
Can I run controlled-impedance traces over a hatch?
You can, but it is the harder path. Keep openings small compared with the trace width, route at an angle to the hatch, keep the pattern uniform along the whole run, and verify on a coupon. If the impedance tolerance is tight, use a solid plane in the static region and confine the hatch to the bend.
Is a hatched plane as good for shielding as solid copper?
No, it is a compromise, but on a fine hatch the aperture itself is usually small compared with the wavelength at typical frequencies. The bigger loss is usually return-path and impedance stability. If you need high shielding in a dynamic bend, consider shielding film instead of a copper plane.
At what angle should I orient the hatch?
Around 45° to the trace direction keeps traces crossing lines consistently, and about 45° to the bend axis avoids a long copper line running parallel to the fold. Agree the exact orientation with your fabricator for your bend geometry.
Should the whole flex board use a hatched plane?
Usually not. Use solid copper where the board is static or in rigid sections, and hatch (or shielding film) only where it flexes. Hatching everywhere gives up impedance predictability across the whole board for a mechanical benefit that exists only in the bend.