ok, this is potentially the final version. Speak now or forever hold your peace:
edit: ignore the airwire on the power connector… fixed that one :)](ImageShack - Best place for all of your image hosting and image sharing needs)
Hi Galed;
The PCB before this last one looked the best so far. The ground plane below the micro strip does NOT need to be extended all the way to the antenna, only up to where the rest of the ground plane ends.
Another option is to use a coplanar waveguide instead of a microstrip. This will allow a narrower trace to get the 50 ohms you need, and will allow you to bring your top ground pour closer to the transmission line itself.
In all reality, your transmission line is very short, so you can screw it up a little bit and still not have significant path loss in practice. Much more important for antenna performance will be the layout with respect to the groundplane, and any objects in the near field.
If you refer to the antenna datasheet, it will show the ideal layout. With these 1/4 wave chip antennas, you need to follow the suggested layout as closely as possible, as the antenna actually uses the ground plane as a part of the antenna element, perse. Changing the antenna layout from the suggested layout even a little bit will very quickly de-tune it and depending on the antenna, can quickly make it useless. (i.e. having the groundplane underneath as Leon mentioned)
Hey Roko, thanks for that reply. Here’s the datasheet for that chip antenna:
http://www.sparkfun.com/datasheets/GPS/ … 006-09.pdf
I don’t have room to put a GND plane 1mm from the 50 ohm trace. That gets too close to the Vcc pin on the GPS module itself(which seems like poor design).
Ultimately this is going to be a tight-quarters, enclosed device. basically what i’m hearing is that i should look into an active antenna.
EDIT:
I’ve decided to go with a coplanar waveguide because I understand it better. I found the following here: http://www.delorme.com/byUse/gpsmodules … Design.pdf
For a two-layer board design, typically 0.062” thick board made with FR-4 material (Dielectric = 4.6) and 1 oz copper (1.2-1.4 mils thick), the RF-input should be 30-32mils wide, the gap to the adjacent grounds should be 6 mils, and each of the RF grounds should be at least twice the width of the input signal (60-64mils).
Is this sound advice? Unfortunately, with batchpcb the smallest spacing available is 8mil. I ran it through a calculator and got 49.75 ohms with .064" FR4 using the dielectric constant of 4.6, spacing of 8mil and a trace width of 68mil. Unfortunately I can’t make the ground on both sides wide enough. And the RF-GND is NOT connected to the digital ground of the circuit at all… This is what results:
How close should the vias be? Keep in mind, the minimum size is 20 mil (i know, that’s big)](ImageShack - Best place for all of your image hosting and image sharing needs)
On an unrelated note to the antenna, it looks like none of your expansion connectors has a ground pin. I’d consider adding one (and maybe even a power pin) to make them more useful.
/mike
Hi Galed;
Some comments:
-
I’d connect GND directly to RF_GND, and not split the ground planes. I’ve seen more problems because of improperly split ground planes than from having planes connected…
-
It looks like you’re making VCC as the top plane and GND on the bottom? For an RF 2 layer PCB, I’d recommend making both top and bottom pours ground, with plenty of vias between the two. This way you can extend the ground on the top layer to the edges of the board to make sure you have a very healthy ground for the chip antenna to work properly, as well as good ground returns. Then route the VCC from the regulator in a star pattern to the different sub-circuits on the board. (There are several schools of thought on this one, but that’s the method I prefer and have had good results with.).
-
Bring the RF GND back a bit to be flush with all the ground plane, on both layers. Then just make sure that the antenna is spaced away from the ground plane as in the datasheet. This will give you as close to the advertised specs on the antenna as you can. It’s okay that the last little bit of the feed line won’t be a proper transmission line, the antenna
should have been designed by to be fed as show in the data sheet.
- Double check the GPS data sheet, but I’m assuming the two pins on the antenna feed line of the GPS module are RF_GND. They should be connected directly to the RF_GND pour beside and below your transmission line. (I.e. connect them on them coming out of the right side of the GPS module). It’s okay if you make a triangle shape for the transmission line to get it from the thickness of the pad to the thickness of 50 Ohm transmission line, in order to get a good ground connection on either side of it.
RF is finicky if you don’t do it right, especially with transmission lines and 1/4 chip/printed antennae, but once you get it close, it’ll work pretty good. 
Thanks again Roko.
-
Done
-
That’s right, VCC on top and GND on the bottom. I’d like to keep it that way if I can
-
Done. HOWEVER, the datasheet appears to recommend 1mm spacing between the 50Ω trace and the ground plane. Because of the position of the VCC pin on this GPS unit, there’s not enough room to do that… Now, the pins on either side of the RFIN pin are GND, the ones on the outside of those have no internal connection, so they can also be grounded, and I end up with a much bigger grounded area on the top layer.
-
The GPS unit itself actually has only one GND, no separate RFGND
OK, big change of plans… I’m gonna use a non-chip antenna. Because this is basically an application-specific development board, I don’t really care. I just need it to work :roll: I’ll probably end up with a helical antenna or a module with the antenna mounted on it eventually, but that’s a few revisions down the line… For now, I’m going to use an external patch antenna hooked up to an SMA edge connector, modeling the GPS modules that SFE sells.