Because of the high maintenance needed to monitor and filter spammers from the RF Cafe Forums, I decided that it would
be best to just archive the pages to make all the good information posted in the past available for review. It is unfortunate
that the scumbags of the world ruin an otherwise useful venue for people wanting to exchanged useful ideas and views.
It seems that the more formal social media like Facebook pretty much dominate this kind of venue anymore anyway, so if
you would like to post something on RF Cafe's
page, please do.
Below are all of the forum threads, including all
the responses to the original posts.
Post subject: 4 layer PCB: third layer?! Posted: Thu Jan 10,
2008 4:40 am
Joined: Thu Jan 10, 2008
I´m new to this forum and
I hope you can help me with my question.
Acutally 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
- 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 to VCC.
any experiences that you can share with me/us? Should one of the options
should be prefered (why?)?
Posted: Thu Jan 10, 2008 3:03 pm
Thu Sep 25, 2003 1:19 am
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 5:38 pm
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, tec.
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.
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 manufacturing.