This is my first attempt in designing a pcb layout for a gps chip antenna. PCB is two layered. All the components (including the antenna) are on the bottom layer. I have assumed it to be a "co-planar wave" transmission line (NetANT_2). The width of the feed line is calculated using the "Saturn PCB design toolkit".

My concern is, can this transmission line be considered as "co-planar wave"? as I think there is no sufficient ground plane to left of the feed line. Really appreciate the help. Thanks.

enter image description here

EDIT: The length of the feed line (NetANT_2) =138mils (3.505mm), width= 33.325mils (0.84mm). The ground plane gap is 8mils(0.203mm). substrate height 0.66mm. U10 is a LNA(MAX2659).

  • \$\begingroup\$ It doesn't appear to be a very long trace with respect to wavelength of the signal but as there are no dimensionsal clues maybe you should fill in the missing detail. Also the effective path through L3 and C38 should also be considered. Is U10 the driving source? One more point of interest - you don't appear to have formally "accepted" answers to any question you have raised and this might be seen as some folk a reason not to provide you with help. \$\endgroup\$
    – Andy aka
    Commented Aug 28, 2016 at 11:06
  • \$\begingroup\$ oh, I did not realize that. I will fill in the details. And also i am truly sorry for not formally acknowledging the help i received. Thanks \$\endgroup\$
    – R. Hirur
    Commented Aug 28, 2016 at 12:00

1 Answer 1


Yes, this can be considered a CPWG and it will do better than a line without tuned impedance.

Your dimensions seem correct for 50 ohm impedance, assuming you are using FR4 with a dielectric constant around 4.5 . The proximity to the board edge should not be a concern.

I think you do not need quite as many fence vias. I would instead suggest to place the signal line passives straight to avoid the angle at C38, or --- as an alternative --- to use soft bends with radii around 3 times the line width.

Be sure to place C37 nearer to the LNAs supply pin and always put double vias to ground on shunt capacitors to avoid issues with via inductance.

  • \$\begingroup\$ Thank you for the reply. I was wondering about the length of the feed line. I know that the characteristic impedance is independent of the length. Is there a thumb rule as to what should be the length of the feed line ? \$\endgroup\$
    – R. Hirur
    Commented Sep 22, 2016 at 15:00
  • 1
    \$\begingroup\$ @R.Hirur The length is not something to optimize for unless you need a specific phase shift. Having the LNA not too far from the antenna will help though. Look for PCB recommendations from the antenna manufacturer. If there is a reference layout, replicate it 1:1 or at least make sure you understand why things are arranged like this. \$\endgroup\$
    – Andreas
    Commented Sep 22, 2016 at 16:14

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

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