Post your RF PCB questions below before May 29th and our experts @steve.carney, @allank, and @atar.mittal will get you the answers!
Why is it recommended to route RF traces on the outer layers? Is it in case of a hybrid stackup? It seems like there are scenarios where sandwiching RF traces inside might be preferred.
How do you calculate the distance between an RF trace and the coplanar ground plane?
You need a simulator. There are a lot of simulators on the market. Many of them are for free, for example in this webpage.
Webpage?
In case of microstrip RF traces with an open mask, a surface finish will be applied during manufacturing. How do we ensure that the additional surface finish does not impact the RF signal impedance?
RF signals are ideally placed on outer layers for several reasons:
-
Speed of electromagnetic waves:
The speed of electromagnetic waves is highest on the outer layers because the effective dielectric constant is lowest in these areas. On the outer layers, the presence of air, which has a very low dielectric constant, further reduces the effective dielectric constant, increasing the signal speed. -
Hybrid stack-up considerations:
In a hybrid stack-up, materials between layers 1 and 2 are usually high-frequency materials like Rogers, which have low dielectric constants (around 2 to 3). This results in higher signal speeds on the outer layers. -
Propagation time:
Reducing propagation time is crucial in high-frequency applications, and the higher speed on the outer layers helps achieve this. -
Core construction stability:
A core construction is often used between layers 1 and 2 in high-frequency RF traces. The core’s thickness remains constant regardless of copper percentage, providing a stable dielectric thickness and dielectric constant. This stability leads to better control over the impedance, making it advantageous to route RF signals on the outer layers.
@eduardo.mateos true.
Use an online calculator or the built-in calculators in EDA tools, as these rely on complex empirical equations. You don’t need to calculate this distance manually. It is recommended not to use a distance of less than 5 mils, with 6 mils preferable.
The decision depends on whether the transmission line’s insertion loss during signal transmission remains acceptable at the highest signal frequency. If so, masking can be used; avoid masking and opt for a suitable surface finish such as gold or tin. A thin gold finish typically does not significantly affect impedance.
2 Likes
let me add more reasons:
No using Vias for Microstrip ;
using a Via for RF conductor as for High Speed Digital will cause reflections and stray capacitance between via and powersupply planes.
the Via impedance cant be controlled by manufacterer as designed by calculator.
the added capacitance “loads” will delay the Signal propagation and change its impedance.
Disadvantages for Microstrip:
the External Layers are exposed to adding 20-30 microns durinng plating process, so the final thicness is not best controlled as inner layers.
The PCB process uses prepreg between layers 1&2 so the final distance between RF conductor and GND Plane is not well controlled too
But using single clad laminate with low loss tangent will be better final distance between layers 1&2
Using Via Fences and grounded coplanar waveguide is a must.
3 Likes
Ok, thanks. Do you have best practices for designing via fences and grounded coplanar waveguides for RF traces? Can you share tips for optimal performance.
Can you recommend specific materials?