What are some good guidelines for positioning a passive chip antenna on a circuit board? Obviously you don’t want any high frequency signals running around near it, but other than that…? Here’s what it looks like now:
the big IC is an ATXMega256A3, below it to the left is an accelerometer. next to that is a microSD card slot. On the top are the USB ports (one as a fake com port for usart debugging, the other to act as a real usb device), the in circuit programmer, the reset button and an 8-pin header for an lcd eventually. On the right is the GPS unit. The antenna is a sparkfun antenna actually, and is on the far right side.
This is the first board I’ve done with an antenna built onto it like this. Should this work?
leon_heller:
Whatever you do, don’t put a ground plane under the antenna! SFE did that once and ruined the range. Don’t run any tracks near it, either.
Leon
thanks for that heads up. good to know.
ok, added holes for standoffs, and got rid of both the vcc and gnd plane under and around the antenna, 'cause that’s what SFE did with their mini-gps eval boards (http://www.sparkfun.com/commerce/produc … ts_id=8936)
Use the sparkfun standoff parts, they look and work much better than what you have.
I would get rid of the ground plane all the way from top to bottom where you can.
Some components (like the 0603s near the antenna) are very close to other parts, I would space everything out a bit as well. Also, use round vias (and maybe smaller ones, those ones look huge).
gussy:
Use the sparkfun standoff parts, they look and work much better than what you have.
I would get rid of the ground plane all the way from top to bottom where you can.
Some components (like the 0603s near the antenna) are very close to other parts, I would space everything out a bit as well. Also, use round vias (and maybe smaller ones, those ones look huge).
Get rid of the ground plane on the right hand side from top to bottom? What about the Vcc plane? and why?
Yeah, those two caps are really close to the GPS unit. Is your worry solderability of the parts or proper functioning with them close together like that?
Why round vias? batchpcb’s minimum drill is 20 mil, so that’s what they all are
leon_heller:
Ideally, the antenna should be connected to the chip via 50 ohm microstrip.
Leon
I don’t have any RF background yet. I’m not entirely sure what that means but i’ll try to figure it out
Where you have already taken out the ground plane, I would extend that further to the top and further to the bottom of the board, not just the small window you have.
My concern of the 0603 passives is solder-ability.
I think others are worrying too much about the 0603 caps being closely spaced - I regularly pack components MUCH tighter than this without issues.
Just a note about the vias: the vias connecting to the groundplane should be very close to the decoupling capacitors. Also, when the ground & power pins being decoupled are close to each other (as is the case here with the microcontroller), and you are only using one via for the ground, the capacitor should be placed between the via and the pin being decoupled.
EDIT: it looks like the ground & power planes are shorted together close to one of the capacitors to the right of the microcontroller.
MichaelN:
I think others are worrying too much about the 0603 caps being closely spaced - I regularly pack components MUCH tighter than this without issues.
So do I, but I know that I can place parts that close, and solder them. Was just making sure the OP realised.
oh, we’re talking about inductive and capacitive impedance from its interaction with the traces around it, not from the resistance of the material. i think i got it…
Here’s what I have now. The whole board got bigger (again) to 2.5" square. Is this the right thing to do for the GPS antenna? It seems strange to me
MichaelN:
I think others are worrying too much about the 0603 caps being closely spaced - I regularly pack components MUCH tighter than this without issues.
Just a note about the vias: the vias connecting to the groundplane should be very close to the decoupling capacitors. Also, when the ground & power pins being decoupled are close to each other (as is the case here with the microcontroller), and you are only using one via for the ground, the capacitor should be placed between the via and the pin being decoupled.
EDIT: it looks like the ground & power planes are shorted together close to one of the capacitors to the right of the microcontroller.
I agree. I've soldered 0603's like this before so these should be no problem.
How crucial is the positioning of the ground via/pin/cap?
I’ll work on getting the vias / capacitors in the right place. Thanks. I see why you say that, but it’s just a graphics artifact. Let me see if i can get a higher resolution image
leon_heller:
The antenna microstrip should have a ground plane underneath the whole track and it shouldn’t be surrounded by copper.
Leon
the bottom of the whole board is a ground plane. And i need to get rid of the VCC pour around the microstrip. Unfortunately, that pin that the caps are on (three down from the microstrip) is the only power pin to the device, so those caps need to be nearby
The positioning of the vias for the decoupling capacitors is more critical the higher the frequency, particulary if you are trying to pass EMC testing.
You shouldn’t have any problems in this regard, but if it was a high-speed FPGA circuit running at hundres of MHz+ it might be another story…
