I understand that the dielectric material on a PCB, such as FR-4, plays a role in determining the capacitance between layers—thinner dielectric materials result in higher capacitance. However, I’m curious about the practical implications of this capacitance. Why is it significant, and in which types of applications or designs should the thickness of the dielectric material be a key consideration?
The capacitance between copper planes in different layers of a PCB is generally smaller than that of discrete capacitors. However, it has a significantly lower parasitic series inductance, making it crucial for high-frequency applications, typically above a few hundred MHz. This characteristic is essential for decoupling fast ICs and handling ESD effectively.
Additionally, the capacitance between a trace and the underlying plane directly impacts the trace’s characteristic impedance. A thinner dielectric layer lowers the characteristic impedance for a given trace geometry. This allows for smaller trace dimensions while maintaining the desired impedance, which is particularly advantageous in dense, high-speed routing scenarios.
1 Like
Replying for the updates.
1 Like
@will has given a great answer. In addition to this it is worth adding that thinner dielectric results in closer proximity of signal to plane which in turn increases the amount of coupling between them and therefore the proportion radiating as unwanted emissions from the board (i.e., EMC radiated emissions) is reduced. In just about every situation, making the trace to plane separation as small as possible helps, and usually the impact is significant.
There is of course one obvious scenario where this does not help: this is where you have to handle very high voltages on the PCB, then the field strength induces breakdown of the insulation. But do the maths and you’ll find the voltage that you can withstand per mm means you can still have really rather high voltages, even when you’re working with prepregs down to 50um or so. When working with very thin dielectrics, remember that the pressing process for adding the external laminations may result in the real thickness after pressing be a little thinner that you might anticipate, so when voltage matters, be generous with the numbers and check with the PCB vendor what the actual minimum thicknesses could be after pressing.
2 Likes
Always great advice from @jonathan.lloyd.riley !
Every dielectric between two conductors, including PCB copper layers, forms a capacitor. The capacitance depends on the conductor area, separation distance, and dielectric properties. In a PCB, thinner dielectrics increase capacitance between planes, and wider traces create larger coupling areas.
This is particularly significant in high-frequency and high-impedance circuits where stray capacitance influences performance. For example, in circuits like oscillators or microcontroller-crystal connections, PCB parasitic capacitance must be factored into load capacitor values to maintain proper operation. Additionally, for radio-frequency boards, specialized materials with tailored dielectric properties may replace FR-4 to optimize performance.
Understanding these effects is critical for designs sensitive to impedance, high frequencies, or parasitic capacitance, helping achieve reliable and accurate circuit behavior.
1 Like