If you need assistance, please send an email to forum at 4hv dot org. To ensure your email is not marked as spam, please include the phrase "4hv help" in the subject line. You can also find assistance via IRC, at irc.shadowworld.net, room #hvcomm.
Support 4hv.org!
Donate:
4hv.org is hosted on a dedicated server. Unfortunately, this server costs and we rely on the help of site members to keep 4hv.org running. Please consider donating. We will place your name on the thanks list and you'll be helping to keep 4hv.org alive and free for everyone. Members whose names appear in red bold have donated recently. Green bold denotes those who have recently donated to keep the server carbon neutral.
Special Thanks To:
Aaron Holmes
Aaron Wheeler
Adam Horden
Alan Scrimgeour
Andre
Andrew Haynes
Anonymous000
asabase
Austin Weil
barney
Barry
Bert Hickman
Bill Kukowski
Blitzorn
Brandon Paradelas
Bruce Bowling
BubeeMike
Byong Park
Cesiumsponge
Chris F.
Chris Hooper
Corey Worthington
Derek Woodroffe
Dalus
Dan Strother
Daniel Davis
Daniel Uhrenholt
datasheetarchive
Dave Billington
Dave Marshall
David F.
Dennis Rogers
drelectrix
Dr. John Gudenas
Dr. Spark
E.TexasTesla
eastvoltresearch
Eirik Taylor
Erik Dyakov
Erlend^SE
Finn Hammer
Firebug24k
GalliumMan
Gary Peterson
George Slade
GhostNull
Gordon Mcknight
Graham Armitage
Grant
GreySoul
Henry H
IamSmooth
In memory of Leo Powning
Jacob Cash
James Howells
James Pawson
Jeff Greenfield
Jeff Thomas
Jesse Frost
Jim Mitchell
jlr134
Joe Mastroianni
John Forcina
John Oberg
John Willcutt
Jon Newcomb
klugesmith
Leslie Wright
Lutz Hoffman
Mads Barnkob
Martin King
Mats Karlsson
Matt Gibson
Matthew Guidry
mbd
Michael D'Angelo
Mikkel
mileswaldron
mister_rf
Neil Foster
Nick de Smith
Nick Soroka
nicklenorp
Nik
Norman Stanley
Patrick Coleman
Paul Brodie
Paul Jordan
Paul Montgomery
Ped
Peter Krogen
Peter Terren
PhilGood
Richard Feldman
Robert Bush
Royce Bailey
Scott Fusare
Scott Newman
smiffy
Stella
Steven Busic
Steve Conner
Steve Jones
Steve Ward
Sulaiman
Thomas Coyle
Thomas A. Wallace
Thomas W
Timo
Torch
Ulf Jonsson
vasil
Vaxian
vladi mazzilli
wastehl
Weston
William Kim
William N.
William Stehl
Wesley Venis
The aforementioned have contributed financially to the continuing triumph of 4hv.org. They are deserving of my most heartfelt thanks.
Registered Member #1062
Joined: Tue Oct 16 2007, 02:01AM
Location:
Posts: 1529
I am working on a 4 layer PCB design, with the stackup as follows: Signal Ground Power Signal
I have a couple of questions. Is there any harm in using multiple voltages on the power layer? the majority will be 3v3, but some will be 5v (power input) and 1v (core supply) that will be routed like a normal route, though with larger areas. Also, what kind of precautions should I take when routing the 20mhz clock signal? Right now it is routed through the bottom layer (8 mil trace), and about .5" in length.
Registered Member #72
Joined: Thu Feb 09 2006, 08:29AM
Location: UK St. Albans
Posts: 1659
Unless you are drawing a lot of current, or relying on widely-spaced shunt capacitors to nail your power for the whole board, you can (and should) treat your power supply as just another signal. 1v will be very intolerant of drops, so use a wide track. My conservative figure for copper is 20mohms, for a 1m length of 1mm2 conductor. Work out your copper thickness and width, and work out the resistance for drops, don't go on the default 1A per mm width default which is valid for temperature rise, not for volt-drop.
Generally, if your total trace length is less than lambda/20 (remember speed of light in PCB ~ 50-60% of c in free space) then you need take no precautions with the sending, trace between them or the recieving end, other than making sure it still calculates to work. Treat the trace as a lumped capacitance which your sender has to drive.
Once your trace length gets to lambda/4, you need to be worrying about termination. Doesn't sound like you're there yet.
Top-side signals only see ground, whereas bottom-side signals can couple with the power layer. Think about whether you want this coupling. Minimise by crossing traces at right-angles.
A very useful board layout techiniaue if you have two layers for routing is to do it "Manhattan" style, one layer goes E-W, the other layer goes N-S, and forget about power and signal layers. That way, using vias, you can always get from one point of the board to another systematically without your route being obstructed by prevously routined traces. Everything's going to couple, so use this pair for power and low quality signals, critical traces go on the top side where they only see ground.
Registered Member #311
Joined: Sun Mar 12 2006, 08:28PM
Location:
Posts: 253
wrote ...
Top-side signals only see ground, whereas bottom-side signals can couple with the power layer. Think about whether you want this coupling. Minimise by crossing traces at right-angles.
A well-decoupled power plane is to all intents and purposes the same as ground for changing signals
wrote ...
A very useful board layout technique if you have two layers for routing is to do it "Manhattan" style, one layer goes E-W, the other layer goes N-S, and forget about power and signal layers.
This is fine for through-hole but doesn't really work for surface mount boards of any reasonable density due to the obstruction caused by part footprints.
Registered Member #1062
Joined: Tue Oct 16 2007, 02:01AM
Location:
Posts: 1529
Thanks for the in depth reply.
Mike is right, I don't think I can keep with that style, I will keep that in mind though. I may end up mounting components on both sides, however critical parts will stay on top. Here is a screenshot of the layout so far. The cyan layer is power (The large cyan polygon is the 1v), and the purple is the ground layer (supply later, so it is inverted). The clock is highlighted. The QFN chip in the middle is 10mm square, and most passives are 0402 for size reference. The entire bottom right block is power regulation, 5v in and 3v3 and 1v out. I still need to add a 1.8v supply for the USB PHY. Any general comments about how I am laying it out? Each PCB run will cost close to $500, so I don't want to have to order 5 revisions...
Registered Member #72
Joined: Thu Feb 09 2006, 08:29AM
Location: UK St. Albans
Posts: 1659
wrote ...
A very useful board layout technique if you have two layers for routing is to do it "Manhattan" style, one layer goes E-W, the other layer goes N-S, and forget about power and signal layers.
This is fine for through-hole but doesn't really work for surface mount boards of any reasonable density due to the obstruction caused by part footprints.
I use it all the time on surface mount boards at work, but then I do use buried vias (even more expense). It's true that if your vias have to go full depth, it rather limits how useful it is.
The present board I'm working on is 10 layer, sig/gnd/sig/gnd with vias 1-4, then 5 and 6 are Manhattan, then gnd, sig, gnd, sig with vias 7 to 10.
Registered Member #1062
Joined: Tue Oct 16 2007, 02:01AM
Location:
Posts: 1529
Should I still put a ground pour on the signal layers? Here is an update: Again, the large cyan pour is 1v. the purple is the invert of the ground layer. Any glaring bad practices?
Registered Member #72
Joined: Thu Feb 09 2006, 08:29AM
Location: UK St. Albans
Posts: 1659
As you have already defined layer 2 as ground, you can leave it at that. Make sure that you haven't routed any last-minute tracks through layer 2, robbing it of continuity.
Don't pour grounds on signal layers (generally).
It is very unusual that it would fix a bad board.
It very common that it can f*c*up a good one.
By all means simplify the placing of additional grounds by outlining the area with a continuous track and pouring into the space. Just don't let it pour round signal tracks. A big area of copper is soometimes useful as a heatsink. Again, place it and delimit it carefully, don't just pour it.
If you need grounds between signals for isolation or impedance control, then put them in manually as tracks. It's too important to lose the control and hope the tools have done what you hoped they have.
This site is powered by e107, which is released under the GNU GPL License. All work on this site, except where otherwise noted, is licensed under a Creative Commons Attribution-ShareAlike 2.5 License. By submitting any information to this site, you agree that anything submitted will be so licensed. Please read our Disclaimer and Policies page for information on your rights and responsibilities regarding this site.
Some PCB layout questions
