RF Trace Impedance for PCB:NG

[kb1lqc]

Referring to PCB:NG's stackup to create 50 Ohm traces for long runs of RF

• [x] Top Layer
• [x] Inner B Layer

[kb1lqc]

Updated RF Routing for Better Isolation

• Red pen Lines show copper pullback for ground pours on same layer as RF routing
• Green pen lines show via fences which also pulled back.

I decided to update the RF routing to get at least 3x the PCB ground reference height from the RF trace to the nearest ground pour on the same layer. While I couldn't hold this everywhere, it's nearly all correct.

PCB:NG uses a 13 mil spacing between the Top Layer and Inner A as well as the same spacing between the Bottom layer and Inner B. The core is 28 mils between Inner A and B. Therefore I should have about 3x13mils = 39mils of copper pullback. I went for 4x and kept about 50 mils to be safe.

Via fences were moved to accomodate as well as clean up their placement. I also moved the ground traces from the SAW filter which were redundant and above the SAW filter to help align the via fence above the CC1190 PA area.

[kb1lqc]

Pulled Back Ground More Near LNA

• I pulled the ground away in the area inside the red pen circle to help protect the LNA.
• The goal was to achieve 50 mils but in some areas I was forced to leave the ground only 7 mils away. However these areas are unavoidable without drastic redesign and frankly not worth it 😄

[kb1lqc]

Inner Layer Impedance

Using Saturn PCB Toolkit I've calculated the necessary trace with of 16.7mils to achieve 50 Ohms on Inner B (Blue) layer.

• Inner A layer above Inner B is solid groundplane everywhere except via holes
• Bottom layer 13 mils away from the Inner B layer is the hard reference and is solid groundplane directly below the RF trace area.

• [x] Inner B layer shows correct 16.7 mil trace width on CC1190 RF section

[kb1lqc]

Top Layer 50 Ohm Trace

Again using Saturn PCB and the PCB:NG stackup I've calculated a nominal 25.6mil trace width for the top or bottom layers (since they are both microstrips with same properties).

• Top or bottom layers hard reference Inner A and Inner B layers respectively
• About 50 mils spacing for ground pour on same layere wherever possible

• CC1190 RF section looks good

• The GPS has a small section with RF traces exiting and immediately reentering the module where I also pulled back the ground pour
• I know it looks a bit wonky but I kept the ground behind the RF pin because the two pads for ground are immediately adjacent to the RF pin 6 so it doesn't really make a difference.
• Achieved 50mil pullback for most of the area.
• [x] RF trace is 25.6 mils with a ground layer on Inner A directly below (white pour)