I'm struggling with specifying the convenient signal wire width for the grounded co-planar waveguide for the following parameters: - PCB: FR4, 1.5mm - copper thickness: 0.035mm - pad to pin lenth: 9.8mm - space between ground and path signal on the same layer: 0.254mm - frequency: 900/1800MHz (GSM modem)

For these parameters KiCad calculator gives me signal track width of 1.28 mm which is more than the pad width (0.8mm). The clearance issue I can solve by simply ending the track lower than the bottom edge of the modem pad so that it does not go between pins 46 and 48 disturbing their clearances but will that solution be ok? The image below shows this solution (no ground aside yet)

The only possible ways of making the signal track narrower is to increase the PCB thickness or making the space to the ground planes aside less, but that on the other hand is a PCB making company constraint (they support 10+ mils)

enter image description here


The easy way:

Keep your design as-is.

The wavelength at 1800 MHz is 167 mm. Your track length is 10 mm. This is less than 1/10 wavelength so you can probably get away with not worrying too much about controlled impedance on this line. Certainly the few mm of necked-down trace at the pad end of your track are not going to be a big problem.

The hard way:

If you use a thinner dielectric, the required trace width will get narrower (certainly for microstrip geometry, probably also for CPW but I haven't double-checked this). You could either switch to something like a 1 mm dielectric thickness to get a slightly narrower trace width, or make a 4-layer board to get full freedom to choose your dielectric thickness. If you go with a 4-layer board, choose the dielectric thickness (of the microstrip/CPW structure) to give you a trace width that matches the pad width.

| improve this answer | |
  • \$\begingroup\$ While you can certainly do plenty of damage with a metal tuning stub that is 1/10th the wavelength of your signal, your overall point is correct. Additionally, a small chamfer or "launch" at the pad output is certainly acceptable no matter what your design. \$\endgroup\$ – scld Nov 26 '13 at 20:24
  • \$\begingroup\$ @The Photon: does that mean that controlled impedance is significant only for signal tracks longer than 1/10th of wave length? \$\endgroup\$ – tml Nov 27 '13 at 18:24
  • \$\begingroup\$ @tml, that's a common rule of thumb. But 1. You still want to maintain a clean return path. 2. If your application is really critical (analog) you might want to be more careful. 3. Trying to get close to the right geometry for controlled impedance is still a good idea. In your proposed layout, those last couple of mm where the track necks down are really unlikely to cause a problem (might even help a tiny bit to balance any excess capacitance on the modem's input pin). \$\endgroup\$ – The Photon Nov 27 '13 at 18:46

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.