When I tried to put Molex GPS ceramic patch antenna 2042860001 on two-layer PCB, I found it's impossible to connect the feed pin to the RF trace on the two-layer PCB if following the recommended layout. As indicated in the recommended PCB layout as below, the feed pin is fully surrounded by the ground copper on both layers which leaves no path for the RF trace. Does this mean for this RF antenna, more than 2 layers are mandatory? If not, how should the feed pin be connected?

enter image description here


1 Answer 1


Yes, Molex's drawing requires a PCB of at least 3 layers. I would use a 4-layer PCB.

It's strange that Molex doesn't say anything about the impedance of the antenna trace that should be 50 Ohm.

If you want to use a 2-layer PCB I suggest you to:

  1. Draw the antenna trace on the top layer. The adhesive sheet suggested by Molex will isolate the antenna from the body of the GPS.

  2. Fill the bottom layer with copper connected to GND.

  3. Fill the top layer of copper connected to GND except for the antenna trace.

  4. Difficult part: antenna width and clearance from the GND copper should be calculated in order to have characteristic impedance of 50 Ohm (*).

  5. Keep the antenna trace as short as possible

  6. Connect together top and bottom layers using a lot of stiching vias on the border of the PCB. Put them on the border and not close to the antenna trace.

(*) Use this free tool. Your trace, as I design it, is a coplanar waveguide trace. You should design it in order to have a characteristic impedance Z0 of 50 Ohm.


That tool supposes that the copper height of your traces is 0.035 mm which is the standard value of 99% of the PCB manufactured on Earth.

  • \$\begingroup\$ Thanks for your comment. To meet the requirements of Molex, I'd like to change the PCB into 4layers. If I set layer stack as follows: layer1- RF signal; layer2 - GND; layer3- Power; layer4 - digital signal, and build the ground wall around the feeding pin on layer1/layer4 as datasheet described, then which layer would be better for the waveguide trace on? The GND or the Power layer? \$\endgroup\$
    – Ross
    Commented Nov 1, 2021 at 22:02
  • \$\begingroup\$ Layer 1: RF and slow signals, Layer 2: GND, Layer 3: Power, Layer 4: signals. Stiching vias connected to GND all around the border create a GND cage that contain spurious RF emissions inside the board. \$\endgroup\$ Commented Nov 2, 2021 at 4:50

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.