PCBs are made out of planes of material. They are stacks of conductive layers sandwiched between insulating layers with plated holes called vias connecting circuitry together on the different conductive layers. Two types of conductive layers are employed: plane layers and signal layers. Signal layers are used for signals, and plane layers are used for power supply voltage rails and for signal return current.
Minimize the separation between signal layers and their reference planes
You want to minimize the distance between signal layers and their reference plane layers, because the loop area of a signal forward path and return current path forms an antenna that produces noise and picks up noise. You want signal paths to be nice and close to their respective return current paths. Return current for a signal on a plane spreads out or bunches up under the forward signal depending on the wavelength or frequency of the signal. Higher frequency components bunch up under the forward signal, and so the return path for high-frequency components needs to be free of obstacles to avoid the return current having to follow some crazy path causing crosstalk and signal integrity problems.
High-Frequency components of return current on a reference plane bunch up under the forward signal
Always Check your return current path
Let’s take a look at an example 4-layer PCB. The layer count refers to the number of conductive (etch) layers in the PCB, and as you can see there are more than 4 layers.
- Silkscreen – Layers of silkscreened text, component reference designators, and markings.
- Soldermask – Insulative layers that is applied over the outer etch layers after they have been plated to protect conductors from oxidation and from unintended solder bridges and short circuits.
- Plating (Surface Finish) – Conductive layer added to the copper etch on outer layers to improve solderability of components and to protect exposed copper.
- Etch – Conductive layer of etched copper. Can be a signal or plane layer.
- Core – Insulative layer that comes premade to the board house with a sheet of copper on one or both sides. Typically Core is a fiberglass material, with FR4 being the most common type.
- Prepreg – Insulative layer that glues Core/copper sheets together. Prepreg is typically a fiberglass material such as FR4 impregnated with resin bonding agent.
- Vias – The plated holes that selectively connect the conductive layers together. The conductive paths for signals to transition between layers.
The thickness of etch layers is specified in copper weight per square foot. Common thicknesses:
- .5 oz copper – 17.5 um, 7 mils
- 1.0 oz copper – 35 um, 1.4 mils
- 2 oz copper – 70 um, 2.8 mils
For plane layers go with 1 oz copper, unless you really need to move alot of current or need low thermal resistance for cooling components in which case go for 2 oz copper. For signal layers, .5 oz copper is typical, or you could do 1 oz copper if you need to share the layer with power distribution.
The characteristic impedance of single-ended traces is determined by the trace width and its distance from neighboring planes, and the characteristic impedance of differential pairs is determined by the trace width, spacing between the pair traces, and distance to the reference plane(s). If you need to implement controlled impedance, there are online trace impedance calculators that can tell you trace width and spacing you need to use in your design, or the best thing is to contact the PCB house who will be building the board, and ask them to give you a stackup model that will hit the controlled impedances you need.
In PCBs characteristic impedance of single-ended signals is usually 50 Ohms. Differential impedance is usually 100 Ohms, with a notable exception being USB which uses 90 Ohms differential. Thanks for that, USB.
Core and Prepreg Layers
Core and prepreg layers are insulators that sandwich the conductive etch layers. There are a few points to keep in mind for Core and Prepreg:
- Thickness of core and prepreg determines characteristic impedance of signals.
- The dielectric constant of the material determines signal propagation speed.
- Safety regulatory bodies require you to use material that is flame retardant: levels 94V-1 or 94V-0. You can ask PCB makers for what’s called a “Yellow Card” for the PCB, which is the safety certificate for the material.
- New regulations may be coming requiring low-halogen materials must be used. (Bromides have been used as fire retardants, but are being restricted.)
The soldermask layer is where you can choose the color of your PCB. A wide variety of soldermask colors are available nowadays.