IMP003 RF Trace Design

Hi all.

I just received the gerbers of my IMP003 design from my PCB designer (see attached, grid is 5mil). The gap between either side of the microstrip antenna feed and the groundplane is a lot narrower than the design guidance however the calculator he used seems to back up the dimensions. Layer stackup is the same as the design guidance. Values entered into the calculator to achieve 50ohm characteristic impedance were: Er=4.2, track width(s)=0.3556mm, gap width (w)=0.1524mm, dielectric thickness (h)=0.2mm.

Has he used the right type of calculator? I note this calculator doesn’t include copper thickness as a parameter. Will this design work?

I’ll leave this to Tom to answer, but generally, it’s the PCB fab which defines this - they will adjust the gerbers to match the required impedance on their specific process. Have you asked the fab for their exact stackup?

Hi Hugo.

I just noticed the file attachment didn’t load, here it is.

My PCB guy advised the stackup is the same as the design guidance.

PCB guy != PCB fab. The fab will adjust the traces, no matter what the PCB designer does.

Your calculator is for a coplanar waveguide with ground rather than a microstrip trace. in a coplanar waveguide the signal is intentionally coupled to the ground on the same layer so it is close. In a microstrip the signal only references the plane below so you have to keep the top ground further back. Both work and each has advantages and disadvantages.

Hi Brandon. Thanks for replying. Interesting read though it sort of adds to my confusion.

The design guidance RF trace, which is identified as a microstrip transmission line, has grounds either side and vias connecting them to the bottom layer. I might be missing something but it looks like a coplanar waveguide yet the trace/side ground dimensions are quite different to those calculated with the coplanar waveguide calculator.

So how is the design guidance microstrip transmission line not a coplanar waveguide and the dimensions so different to those calculated?

With a microstrip there will always be some other traces on the top layer so it’s never perfectly ideal. Since we don’t want other signals coupling onto the rf trace we shield the trace with GND as much as possible. Since we don’t want it to have a significant impact on the impedance we keep it back ~21 mil (don’t remember exactly what we did on that particular stack up, but typically you want at least 3x your dielectric thickness) at which point the lateral coupling is extremely small and so has a very minimal effect. In your stackup, the GND plane is only 7mil below the trace and it couples to the wide part of the trace (width) rather than the short part (thickness) so that will be the dominant factor in determining the impedance.

As Hugo notes, the nice thing about doing a microstrip transmission line is that each Fabrication house knows what trace thickness will get you 50Ω for their exact stackup. This allows them to account for variation in the type of FR4 used, the copper plating thickness, etc. By building a big wide shielding channel for the trace to run though, they can just change the width of the trace without needing to change the GND copper pull back or stitching vias. Typically the way this is done is by making the trace width close to what you think it should be and a strange value like 5.652mil and then in your fab notes you will call out that all 5.652mil traces should be impedance controlled to 50Ω according to the fab house’s specifications.

It’s also worth noting that for a trace this short, it probably doesn’t matter a ton as long as you are close to 50Ω.

Ah, it all makes sense now, thanks Brandon.