Three planar transmission line types cover most RF board designs. Each has trade-offs.

Microstrip
- Trace on an outer layer over a ground plane.
- Easy to fabricate, probe and tune; components mount directly on the line.
- Part of the field is in air, so the effective permittivity is between 1 and the substrate Dk; the line is slightly dispersive.
- Radiates more and is more susceptible to coupling than buried lines; solder mask changes its impedance.

Stripline
- Trace buried between two ground planes in a homogeneous dielectric.
- Excellent isolation and a pure TEM mode (no dispersion from mixed dielectrics).
- Needs vias to transition to components, and the vias need careful design (stubs, anti-pad sizes, ground return vias).
- Narrower trace for the same impedance and stack-up, so conductor loss can be higher.

Grounded coplanar waveguide (GCPWG)
- Trace with coplanar ground on both sides, plus a ground plane below, stitched with vias.
- Good isolation on an outer layer, low radiation, convenient for connectors and probing.
- Impedance depends on both the gap and the dielectric height, giving flexibility.
- Requires disciplined via fencing; poorly stitched side grounds can support unwanted modes.

Design notes
- Use a field-solver-based calculator and the fabricator's actual stack-up, including copper thickness and final Dk at your frequency.
- Ask your fabricator for impedance control and test coupons.
- Account for etching tolerance: a small change in trace width matters for narrow lines.
- Loss has two parts: conductor loss (copper roughness matters) and dielectric loss (dissipation factor Df). Low-loss laminates matter more as frequency and line length increase.

For most multi-GHz boards, GCPWG on the top layer for RF and stripline for sensitive routing is a robust combination.