Copyright: 1996 - 2024
BSEE - KB3UON
RF Cafe began life in 1996 as "RF Tools" in an AOL screen name web space totaling
2 MB. Its primary purpose was to provide me with ready access to commonly needed
formulas and reference material while performing my work as an RF system and circuit
design engineer. The World Wide Web (Internet) was largely an unknown entity at
the time and bandwidth was a scarce commodity. Dial-up modems blazed along at 14.4 kbps
while tying up your telephone line, and a nice lady's voice announced "You've Got
Mail" when a new message arrived...
All trademarks, copyrights, patents, and other rights of ownership to images
and text used on the RF Cafe website are hereby acknowledged.
My Hobby Website:
4 layer PCB: third layer?! - RF Cafe Forums
RF Cafe Forums closed its virtual doors in 2012 mainly due to other social media
platforms dominating public commenting venues. RF Cafe Forums began sometime around
August of 2003 and was quite well-attended for many years. By 2010, Facebook and
Twitter were overwhelmingly dominating online personal interaction, and RF Cafe
Forums activity dropped off precipitously. If the folks at
phpBB would release a version with integrated
sign-in from the major social media platforms, I would resurrect the RF Cafe Forums,
but until then it is probably not worth the effort. Regardless, there are still
lots of great posts in the archive that ware worth looking at.
Below are the old forum threads, including responses to the original posts.
|-- Amateur Radio
Gripes & Humor
-- CAE, CAD, &
Test & Measurement
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.