15
\$\begingroup\$

I've designed a PCB in Eagle to host a GPS Receiver module and a GPS patch antenna. The RF input to the module is specified as a 50Ω unbalanced (coaxial) RF input. I used this calculator to calculate the required width and spacing for a co-planar wave-guide transmission line, and as you can see I got pretty close to 50Ω characteristic impedance using parameters from here. I ended up with a 32 mil trace width and 6 mil separation. Does that seem reasonable?

Here is a screen capture of what my board looks like:

enter image description here

Both the area fills (top and bottom) are GND, and I stitched vias approximately every 75 mil intervals between the top and bottom ground planes all around where the patch antenna is placed and along side the antenna feed to the GPS module. I didn't have any guidance on how to do this properly, so I just kind of eyeballed it. Perhaps it's overkill? I also stopped the top-side ground plane short of the chip to follow guidance that there should be no traces or solder mask under the GPS module.

The inner solid line square is 25mm and represents the actual patch antenna footprint. The dashed line around the patch antenna is a 27mm square that represents the required ground plane under the antenna, as I read it's datasheet. The feed length is about an inch (which is much less than the wavelength at 1575.42MHz) so I don't think path loss is of any concern here. I rounded the feed path it to "avoid sharp corners." I reckon that doesn't really matter too much, but I figured I may as well. Finally I used a 0.9mm drill size for the antenna pin, which I intend to solder on the back side. Does that all seem sound?

If I haven't given adequate background information in some regard, please let me know in a comment and I am happy to add information as necessary if I can. Just looking for an objective review as these are topics that I don't consider myself an expert in, and I can't think of a much better place than here to find knowledgeable and helpful colleagues.

UPDATE

I added a bunch of "random" vias within the ground stitching region under the patch antenna per @Dave's suggestion. Here's an updated board screenshot:

enter image description here

\$\endgroup\$
3
  • \$\begingroup\$ If you could recommend a good method for designing patch antennas that would be really cool. Hey, then i could double check your design!!! \$\endgroup\$
    – Andy aka
    Mar 25, 2013 at 22:39
  • 1
    \$\begingroup\$ @Andyaka my method for designing patch antennas is to buy them ;) \$\endgroup\$
    – vicatcu
    Mar 26, 2013 at 13:38
  • 1
    \$\begingroup\$ a very pragmatic approach!! \$\endgroup\$
    – Andy aka
    Mar 26, 2013 at 13:52

1 Answer 1

Reset to default
5
\$\begingroup\$

It looks pretty reasonable to me. I've got a question and a comment.

What are the components between the antenna and the GPS module? Any clocks etc? If they are power supply lines, it looks a little light on bypassing.

I'd also drop a dozen or so ground vias under the antenna itself, placed randomly. The reasoning behind this is to make sure you don't create a resonant cavity under the antenna, with the walls formed by ground planes top and bottom, as well as the via holes running around the outside. Unlikely, as your pcb is likely to be lossy, but you'd hate to hit the jackpot with that.

\$\endgroup\$
3
  • \$\begingroup\$ They would appear to be decoupling, and a connector carrying only power and reset. Looks fine do me. +1 for avoiding an accidental cavity. \$\endgroup\$
    – user16324
    Mar 26, 2013 at 9:26
  • \$\begingroup\$ The only things between the patch antenna and the GPS module here are two 100nF capacitors for bypass decoupling on the VBATT and 3.3V inputs to the receiver module supply inputs. The header pins between the module and the antenna are to connect an external reset, and to bring in VBATT and 3.3V to the board. \$\endgroup\$
    – vicatcu
    Mar 26, 2013 at 13:39
  • \$\begingroup\$ I added random GND stitch vias per your suggestion and added an updated screen shot to the question under the heading UPDATE. \$\endgroup\$
    – vicatcu
    Mar 26, 2013 at 15:01

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