emo Post subject: Mixed Signal PCB Layout Posted: Wed Jun 07, 2006
12:58 am Lieutenant Joined: Wed Jun 07, 2006 12:38 am
Posts: 4 Hi all! I am a newbie to rf design and I am currently
working on a 4 layer mixed signal PCB layout that includes 2.4GHz transceiver.
The layer stackup is signal-ground-power-signal. The questions I
have are are in regards to (copper fill)grounding. 1. What is
the advantage of using ground (copper fill) on top layer and stitching
it to other ground plane? Should I use this approach? 2. Should stitching
extend to non-RF (digital) sections of the PCB? 3. Why are stitching
vias usually more densly populated in some areas than in others?
Thanks in advance! Top IR Post subject: Posted:
Wed Jun 07, 2006 9:22 am Site Admin Joined: Mon Jun
27, 2005 2:02 pm Posts: 373 Location: Germany Hi emo,
I hope that you placed the RF signals in the top layer and the Digital
signals in the bottom layer. A good advice is to fill as much as possible
the power layer with coppr planes and stitch them to GND. Ground
fill is usually done around the RF signals of the PCB. This is part
of the co-planar transmission lines. You should use this approach. The
advantage is that it reduces the impedance of the ground return and
makes a continuous and complete GND plane. You can extend it
also to Digital sections as much as the layout allows you. The
vias are more densed in the RF sections because the wavelength is smaller.
There is a rule-of-thumb that the space between the vias should not
exceed 1/10 of the signal's wavelength. _________________
Best regards, - IR Top checkz Post subject:
yes, i could not agree morePosted: Thu Jun 08, 2006 4:16
am It is an useful suggesition and i can learn a lot. thanks
IR Top emo Post subject: Posted: Fri Jun 09,
2006 1:58 am Lieutenant Joined: Wed Jun 07, 2006 12:38
am Posts: 4 Thanks for your reply IR! It helped a lot, but I
still have some mor equestions. I did placed RF on top and digital
on the bottom layer. You mentioned that I should fill as much as possible
of power plane with copper and stitch to ground. Did you reffer to filling
top layer (RF) with copper here, or am I missing something? I have
one other question. Do you recomend using continious power plane
or routing power on the power plane using wide traces? I have found
lots of conflicting recomendations in regards to this. Best Regards!
Top IR Post subject: Posted: Fri Jun 09, 2006 7:00
am Site Admin Joined: Mon Jun 27, 2005 2:02 pm
Posts: 373 Location: Germany Hi emo, You are most welcome!
I recommend to use wide power traces and to fill all the gaps between
them with coppoer planes and stitching them to GND with vias.
The copper planes on the top layer are the GND, and they should
be stitched with vias to the copper planes in the power layer.
If you have more questions, please post them or email them to me.
Good luck! _________________ Best regards,
- IR Top Stephen Post subject: Alternative thoughtPosted:
Wed Jun 21, 2006 9:06 pm Captain Joined: Wed Jun 21,
2006 8:33 pm Posts: 21 Location: Queen Creek, Arizona Regarding
the comments, I would like to add that depending on the nature of your
power delivery/power requirements of the system, you would could be
better off using a power plane as opposed to traces. Power delivery
can suffer many of the impedance issues experienced by return paths
in the ground planes. Power planes can be used just like ground
planes for transmission lines assuming there is adequate decapping between
the two(this is great if you are routing lots of digital signals on
the bottom layer as then you would not have issues with signals running
over broken planes). You also avoid problems with manufacturability
by having paired solid planes (though ground filling a power plane would
go a long way toward this goal.) Parallel planes also add a certain
amount of intrinsic decap with very little series inductance.
Just thought I would add my 2cents. _________________
CMOS RF and Analog ESD Specialist! www.srftechnologies.com
Top emo Post subject: Posted: Wed Jun 28, 2006 11:02
pm Lieutenant Joined: Wed Jun 07, 2006 12:38 am Posts:
4 thanks for your help guys! I have yet one more question.
My digital section seems to be more complex than oiginaly intended
so it seems impossible to route only on one layer. I tried to keep all
of the digital signals on botom and RF on top layer, but it is not practical
for this design. Is it ok to route some parts of digital signals
on the top plane (dedicated to RF), or should I use another layer for
this? Thanks again! Top IR Post subject:
Posted: Thu Jun 29, 2006 5:44 am Site Admin Joined:
Mon Jun 27, 2005 2:02 pm Posts: 373 Location: Germany Hi emo,
Yes many times that happens. Try to route on the top layer the digital
signals which have the lowest frequency or with low activity on it.
In this way the RF signals will stay relatively clean. Try also to keep
(As much as possible) a distance between the Digital signals to the
RF signals. Another question: How have you finally routed the
signals by planes or by wide traces? Hope this helps!
_________________ Best regards, - IR Top
emo Post subject: Posted: Thu Jun 29, 2006 12:53 pm
Lieutenant Joined: Wed Jun 07, 2006 12:38 am Posts: 4
I have routed power using thick traces and filled the remainder
of plane with coper connected to ground. i will stich all the grounds
together. Thanks again, your advice helped me a lot!
Top Stephen Post subject: Posted: Thu Jun 29, 2006 12:58
pm Captain Joined: Wed Jun 21, 2006 8:33 pm Posts:
21 Location: Queen Creek, Arizona Emo, IR is correct. It is
perfectly legitimate, just use those digital signals with the lowest
frequency components/activity. Note, this is truly dependent on the
risetime of the digital signals, and then the activity factor.
To use a very crude hypothetical example, a 32kHz Clk with a 3nS
risetime can have strong energy components upto and including 166Mhz.
A 1Mhz Clk with a 10n risetime would have most of its energy under 35Mhz.
This is a crude example so nobody hold me to it, but I think the point
regarding being aware of the risetime of your signals is evident when
deciding which signals to route on the upper plane. One reason also
to be aware of this is that the faster risetimes will generate higher
peak currents in the return path of your ground plane, allowing coupling
to any RF signals sharing that plane. One trick I have used,
if appropriate, is I in somecase I applied a risetime filter to certain
low frequency control signals that were being implemented in ECL logic
(ergo they had very fast risetimes by design). As I did not need the
fast risetime for any spec of the system, by filtering it at the signal
driver, I was able to keep much of my system noise down. This is if
it is appropriate, I do not recommend that people start filtering digital
signals left and right, imagine the board cost and space...ouch.
Ok, I will stop there. stephen _________________ CMOS
RF and Analog ESD Specialist! www.srftechnologies.com
Posted 11/12/2012
|