4 Layer PCB: Third Layer?! - RF Cafe Forums
Post subject: 4 layer PCB: third layer?! Posted: Thu Jan
10, 2008 4:40 am
Joined: Thu Jan 10,
2008 4:05 am
I´m new to this
forum and I hope you can help me with my question.
I´m desinging a rf-board with a 2.4ghz transceiver. I found some
application notes from different suppliers and I found some differences
regarding the layer build up of a four-layer-pcb:
- The first
and fourth layer are almost everytime used for routing with covering
copper (connected to ground) at the remaining space.
- The second
layer is complete ground.
- Regarding the third layer I found
a difference: One company suggests that the third layer is used
for power routing and covering the remaining space with copper connected
to ground. Another suggestion is to add a complete copper-area connected
Are there any experiences that you can share with
me/us? Should one of the options should be prefered (why?)?
Post subject: Posted: Thu Jan 10,
2008 3:03 pm
Joined: Thu Sep 25, 2003
I've always been
told to route layer 3 with power and pour the remaining area with
copper ground. ( for RF boards )
Post subject: Posted: Wed Jan 30, 2008
Joined: Wed May 16, 2007 4:16
In the past, I would make the first inner layer
a ground plane and the second layer a power plane. I do it different
now, and I think that the new way is better.
On the first
inner layer, I create small power planes under the RF chips. If
I need to expand them a little to cover the bias inductors, I will.
Then I connect these separate planes using 40 mil traces to a single
trace outside of the RF area that provides power. This distributed
power method ensures that I am able to isolate power supplies at
RF to eliminate problems with spurious radiation, unwanted oscillation,
The important part is to leave the area under the discrete
components open for the most part on the first inner layer. The
only other thing I would do on that layer is to put a small ground
plane under the RF switch if there is one.
Then, on the
second inner layer (or layer 3 as you call it), put a solid ground
plane under all of the RF circuitry. Stitch it to the top layer
ground connections liberally with vias. Then, on the bottom layer,
pour a ground plane under the RF section so that it fills all of
the area not occupied by other traces.
So why put the ground
plane on layer 3 instead of 2, which is the common wisdom today?
Well, the answer is parasitic capacitance. The layer stackup used
by different board manufacturers varies widely from one to another.
So the gap between the top layer and the layer 2 can be smaller
than you intend. If it is too small, you will get unwanted capacitance
to that big ground plane which will make tuning your TX and RX paths
a pain. You can of course try to specify the buildup and hope your
manufacturer complies. But as things continually move to China,
you are dealing with an unknown there.
So I say why leave
it to chance. By moving the ground plane to the 3rd layer, you ensure
that parasitc capacitance for any common layer stackup won't be
a problem. Your circuits will be easier to tune and will work better,
and you will have less problems moving your product to China for