In my design I use GPS module u-blox MAX-7, LNA MAX2659 and chip GPS antenna. First prototype design shows good signal strength, in 2 minutes from a cold start I have a fix. Here is the picture of PCB layout: Old design

The highlighted trace is RF signal from LNA to GPS module. Under this section, there is LCD display (U7).

Now, I had to significantly modify the PCB layout, because I changed some parts(LCD, GPS antenna etc.) and I want to fit the device into a small enclosure. The size of PCB is very limited, so I came up with this design:

New design

As you can see, because of size limitation I moved the GPS module to the bottom layer of PCB and I had to use via to route the RF signal to the module. Again, there is LCD display next to this section.

My problem is that now the signal I get is really low. I get one message every few seconds. Can via in RF signal route attenuate the signal so much? Do you have any suggestions how to solve this?

PS: I also tried to populate PCB with GPS related parts only. Result was the same.

  • \$\begingroup\$ If i'm following it right in the 2nd layout you have a lot less clearance from the ground plane, I'd almost wonder if that's the bigger problem. \$\endgroup\$
    – PeterJ
    Aug 24, 2014 at 8:30
  • \$\begingroup\$ Trace width and clearance (among other things) determines the impedance of trace, which should be 50 ohm for the best performance. I used application AppCAD to calculate this values. Here is a caption from datasheetof GPS module: "The impedance of the antenna connection must match the 50 Ω impedance of the receiver. To achieve an impedance of 50 Ω, the width W of the micro strip has to be chosen depending on the dielectric thickness H, the dielectric constant εr of the dielectric material of the PCB and on the build-up of the PCB." \$\endgroup\$
    – Rainy
    Aug 24, 2014 at 9:15
  • \$\begingroup\$ What does it say in the data sheets about the performance differences between the two antennas? \$\endgroup\$
    – Andy aka
    Aug 24, 2014 at 10:05
  • \$\begingroup\$ I wasn't thinking of the clearance from the stripline impedance point of view, I meant presumably the antenna should be clear of the ground plane somewhat for proper operation. Most chip antennas I've seen seem to have pretty clear recommendations in that area. \$\endgroup\$
    – PeterJ
    Aug 24, 2014 at 10:09
  • 3
    \$\begingroup\$ In general, RF + vias-in-trace is a giant NO-NO. Can't you put the antenna on the bottom of the board as well? \$\endgroup\$ Aug 24, 2014 at 10:58

1 Answer 1


You need to be more careful with your microstrips. They must be sized based on the thickness of your board and the dielectric you're using (FR-4). The first board probably worked OK because your microstrips were relatively short (and as Connor mentioned, you didn't have any vias). I would recommend a few things:

  • Move all RF components onto the same layer.
  • Make sure there's clearance around the microstrips. It looks like you're pouring a ground plane right next to your RF stuff without any regard to impedance. Because it's difficult to calculate microstrip impedance when you've got a ground plane below and ground planes on the side, I typically pull the same-layer ground planes away by 15-25 mil, just to minimize their effects on the microstrip.
  • Short microstrips are happy microstrips. The longer your feed lines are, the more that parasitic impedances and capacitances on your board alter the line impedance.
  • Treat your microstrips as first-class citizens. Position components and do routing to shorten their length and reduce turns -- even at the expense of all other signals. For your first board, your GPS receiver probably should have been rotated left by 90 degrees, with the LNA RFOUT pin sitting right next to the receiver's RF IN pin. It looks like you treated the RFOUT and the SHDN pins with equal routing priority; don't do that.
  • Hard-right routing is a big no-no. 45 degree miters are better, but for best results, use arcs with a radius at least three times the trace width if at all possible.
  • You have the right idea with via walls. Keep doing that.
  • \$\begingroup\$ As a side note, chip antennas are very sensitive to GND plane shape and size. Also, your case material can be of concern. \$\endgroup\$ Aug 28, 2014 at 1:12

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.