Copper weight, stack-ups and impedance

Three things set the electrical and thermal behaviour of a board beyond its layout: how thick the copper is, how the layers are arranged, and how far each layer sits from its neighbours. This article explains each, and when you need to tell the factory about them.

Copper weight

Copper thickness is given as weight per area: ounces per square foot. One ounce of copper spread over one square foot is about 35 micrometres (0.035 mm, or 1.4 mil) thick. Two ounces is about 70 µm.

1. Copper thickness: the same track at three weights.
2. The insulating laminate under the copper.
3. Etching cuts sideways as well as down, so thick copper leaves wider track bases and needs wider gaps.

Two things are easy to miss:

• Outer layers gain copper in plating. A board ordered with "1 oz" outer copper is usually made from thinner foil, then plated up with copper, because the holes must be plated. The finished thickness is stated differently by different makers; ask whether the figure is the starting foil or the finished copper.
• Thicker copper needs wider gaps and wider tracks. Etching goes sideways as well as down, so heavy copper needs more space to be etched cleanly. Heavy copper also changes how the factory sets the minimum track and gap. Do not design 3 oz copper with the gaps you would use for 0.5 oz.

How much current can a track carry

The current a track can carry depends on its width, the copper thickness, the temperature rise you accept, and whether it is on an outer layer (cooled by air) or an inner layer (not). The standard reference for this is IPC-2221, which gives curves, and its newer companion IPC-2152 is considered a better source. Use a calculator based on them, add margin, and treat results for inner layers more carefully. For a track carrying more than a few amps, consider a wider track, a polygon pour, extra copper weight, or solder-reinforced copper, not a thin track pushed to its limit.

Stack-ups

A stack-up is the ordered list of layers and what lies between them: copper, dielectric thickness and type, copper, and so on. Every multilayer board has one, and the factory decides the actual one unless you specify it.

1. Two layers: copper, one core, copper.
2. Four layers: outer copper, prepreg, inner copper, a core, inner copper, prepreg, outer copper.
3. Six layers: two cores and three layers of prepreg between six copper layers.
4. Prepreg: glass cloth with partly cured resin, which melts and bonds the layers when the board is pressed.
5. Core: a rigid laminate with copper on both sides.

Two layers

Copper on both sides, one core between. Simple and cheap. Good for simple digital, low-speed and many analogue designs.

Four layers

The most common step up. A usual arrangement:

1. Signal (top)
2. Ground plane
3. Power plane (or second ground)
4. Signal (bottom)

The solid ground plane under the top signals gives a return path for the current and keeps the loop areas small, which helps both noise and emission. The inner layers are 0.5 oz or 1 oz copper. A board of 1.6 mm total thickness is the usual case, with the outer dielectric thin (so the top signals sit close to the ground plane) and a thicker core in the middle.

Six layers

A common arrangement is signal, ground, signal, signal, power, signal, or signal, ground, signal, power, ground, signal. The idea is that each signal layer has a plane next to it, and the planes are close to each other where possible. Six layers allow faster signals, a denser layout, and better separation between noisy and quiet parts.

Symmetry

Keep the stack-up symmetric about the centre in both copper amount and dielectric thickness. An unbalanced board bows or twists when heated in reflow, and a bowed board is hard to assemble. If the copper on the top is mostly ground fill and the bottom is empty, add fill to balance.

Controlled impedance

A track on a board behaves as a transmission line. Its characteristic impedance, in ohms, depends on:

• the track width,
• the distance to the reference plane (the dielectric thickness),
• the dielectric constant (Dk) of the material,
• the copper thickness,
• for differential pairs, the gap between the two tracks.

The drawing shows the dimensions you can see. Copper thickness and the dielectric constant of the material count as well.

1. Track width.
2. Height of the insulator between the track and its reference plane.
3. Gap between the two tracks of a differential pair.
4. The reference plane: a solid copper layer under the tracks. Keep it unbroken.

When a signal travels fast enough, a mismatch between the track's impedance and that of the driver and the receiver causes reflections. Whether this is a problem depends on rise time and track length, not only on the clock frequency.

When it matters

You need controlled impedance for interfaces whose standard demands it. Typical targets:

• 50 Ω single-ended for many radio and fast single-ended signals,
• 90 Ω differential for USB,
• 100 Ω differential for Ethernet and for many LVDS, HDMI and DDR-type pairs,
• 85 Ω differential for PCIe is commonly quoted.

Check the target in the datasheet or the standard for your interface, since values differ between versions and designs.

You do not need it for slow signals, for typical GPIO, or for power. Asking for it when you do not need it adds cost.

What the factory needs

• A stack-up. Layer order, copper weights, dielectric type and thickness, and total thickness. The factory's engineers may suggest one that fits their materials.
• Which tracks, on which layers, with what target impedance. For differential pairs, say which tracks are the pair.
• The tolerance you accept. Ten percent is a usual figure. Tighter costs more.
• How it is verified. Factories place test coupons on the panel's edge and measure them; the board itself is not measured. Ask whether you receive a report.

Track width and gap are then adjusted by the factory's engineer to reach the target on the real stack-up, which is why you must accept that your drawn width may change by a small amount.

Calculation

Field solver tools in design software and free online calculators give a good first estimate. The factory's own figure for Dk and thickness is the one that counts, since the nominal values on a data sheet differ from a pressed board.

Practical advice

1. Ask for the factory's standard stack-up for the layer count and thickness before routing.
2. Route impedance-controlled tracks only on layers the stack-up describes.
3. Keep reference planes unbroken under fast signals.
4. Do not mix copper weights on one layer without telling the factory.
5. State what is critical in a short note, not only in the drawing.

How this shows up when you order here

If you order impedance control without a stack-up, the check says so: "impedance control needs a stack-up" is one of its 25 checks. The check cannot tell from the files that a track needs controlled impedance, or whether your stack-up fits your design; say which tracks and which targets with the order. The materials and the stack-ups available are on the capabilities page, and an engineer confirms the details with the order. For materials, read PCB base materials.