# Why does a 4 layer PCB board significantly reduce the trace Width needed for a 50 ohm transmission line when compared to a 2 layer PCB board?

I am designing my first 50 ohm impedance trace on a PCB that connects to a single wire antenna. I was playing around with JLCPCB's impedance calculator and I noticed a significant reduction in the trace width with a 4 layer board when compared to a 2 layer board as you can see in the pictures below:

2 Layer Board:

4 Layer Board:

I know the values that make the biggest difference are trace width, trace thickness, trace type, dielectric constant, and dielectric thickness.

The only thing that changes between these 2 are the amount of layers on the board. That means trace thickness (1 OZ Outer Copper Weight) and trace type (Single Ended (Non coplanar) are the same, dielectric constant changes from 4.5 to 4.6 as seen here, and dielectric height could change because we are going from 2 to 4 layers.

Since dielectric thickness is the only one that changes, does the dielectric thickness really make that big of a difference that it could decrease the required trace width by nearly 2.5mm? Is there a way to find the dielectric thickness in a JLCPCB 4 layer and 2 layer board? Because I have not been able to find the actual dielectric thickness and JLCPCB only gives the finished board height.

An important factor in controlling trace impedance is its distance to the ground plane under it (not the entire PCB thickness, as I think you may be thinking).

With a 2-layer board, you typically have a much thicker dielectric (57 mil in your example). On a 4-layer board, notice the prepreg (dielectric) layer is only 8 mil.

This image is from Saturn PCB Design's PCB Toolkit program:

Note the "H" dimension in the diagram, which is the dielectric thickness.

You said:

Because I have not been able to find the actual dielectric thickness and JLCPCB only gives the finished board height.

Your examples show the thickness of every layer (green box):

"Prepreg" and "Core" are both dielectric, and it's the thickness between signal and its immediate ground plane that matters.