Pick a layer and stick with it

One of the nice things about newer, faster busses like DDR3 and DDR4 is on-die termination.  They are nice because you don’t have a bunch of components clogging up your routing layers, and I would say more importantly, it limits your required layer transitions which can help make your boards quieter.  So take advantage of the fact that you don’t have to route out to a terminator and try to keep your layer transitions limited to underneath the IC.  The area under the IC is a particularly exciting location on the board, and also happens to be the best place for layer transitions.

In a recent aricle in Printed Circuit Design and Fabrication Magazine, I discuss the EMI problems associated with layer transitions.  The article can be found here: http://pcdandf.com/cms/component/content/article/171-current-issue/9656-designers-notebook
Bascially, a stitching via is needed anywhere you transition a signal between layers, to provide a continuous return current path for the signal.  I have discussed return current paths in several previous blogs, but to summarize, broken return path = radiating signal.  This is why a stitching via is needed when a signal transitions between layers.  Well, more precisely, a stitching “thingy” – in the case that the different return paths are planes with the same voltage (usually ground), a via will work.  But if they are at different potentials, a capacitor should be used.  Where on the board are there the most vias and capacitors?  Just around the IC.  This makes it the best place to do any layer transitioning.

Post Author

Posted January 7th, 2013, by

Post Tags

, , , , , , ,

Post Comments

3 Comments

About HyperLynx PCB Analysis Blog

How do you stay up-to-speed with the latest high tech toys, applications, and design trends?

The HyperLynx team will give you tips on electronic circuit simulation software and tools to help solve your most critical needs!

HyperLynx PCB Analysis Blog

@MentorPCB tweets

Follow MentorPCB

Comments

3 comments on this post | ↓ Add Your Own

Commented on March 4, 2014 at 5:54 am
By Donald Acker

I have a question about Vert. Ref Plane Signal/Signal errors. If a trace is routed on layer 1 uses a via to get to layer 3 with a ground layer between them on layer 2, why is this an Error? Will not the return current still travel on layer 2 and therefore not be an Error? If this is true how can I make HyperLynx not treat this as an Error? The stackup is a 6 layer board: Top, Gnd, Sig1, Sig2, Pwr & Bottom.

Commented on March 4, 2014 at 5:58 am
By Donald Acker

I made a mistake, this is an 8 layer board: Top, Gnd1, Sig1, Pwr, Gnd2, Sig2, Gnd3 & Bottom.

Commented on September 3, 2014 at 2:09 pm
By Patrick Carrier

Hi Donald–
The issue is that when you transition to Layer 3, you are actually now referencing BOTH Layer 2 and Layer 4. If you check out my blog from 10/10/12 (and the referenced article), I talk about this in more detail. At high frequencies, when the signal is propagating, it has no idea what a plane is connected to. It will couple onto whatever the nearest “hunks” of metal are – planes and traces (which causes crosstalk) – as they represent the lowest-impedance path for the signal. So for your signal on Layer 3, it is now coupling energy onto both Layer 2 and Layer 4, so there must be some connection between Layer 4 and Layer 2 near that signal via to allow for a continuous return path for the percentage of return current which is now on Layer 4. If those planes are at different potentials, a stitching cap must be used. Actually, a number of stitching caps are best to give you a low-impedance path across a range of frequencies. This is why I was advocating “picking a layer and sticking with it”, since you are effectively making any “layer changes” right at the IC where there tend to be a number of caps already.

Add Your Comment

Archives

September 2014
  • The Future of Integrity
  • An Integrity Cocktail – Mixing SI and PI
  • SI and PI – two flavors of Integrity
  • July 2014
  • Back side cap mounting
  • May 2014
  • Does trace width matter much?
  • January 2014
  • How to connect a capacitor?
  • What capacitor values do I use?
  • July 2013
  • Which do I choose – simulation or measurement?
  • June 2013
  • Correlating simulation and measurement
  • Simulation and measurement
  • February 2013
  • Developing Confidence in Your Analysis Tool – HyperLynx 9.0 Demonstration
  • January 2013
  • Introducing HyperLynx 9.0: Fastest time to accurate results
  • How much stitching do I need?
  • Pick a layer and stick with it
  • Manage reference plane changes for quiet boards
  • October 2012
  • Return current on a stripline
  • Is it ever okay to cross a plane split?
  • EMI problems are easier to fix than you might think
  • July 2012
  • When to remove via stubs and non-functional pads?
  • Process of via design and verification
  • June 2012
  • Got integrity?
  • Impedance
  • What to analyze?
  • Don’t let your board heat up your ICs
  • Put your charts away
  • Co-simulation gets you the real answer
  • May 2012
  • Need stitching vias?
  • Turn off your phone!
  • Is it SSN or is it Crosstalk?
  • Crosstalk is everywhere
  • April 2012
  • The cure for sick waveforms
  • March 2012
  • Running at 6GHz with your eyes closed can be scary
  • It’s never too late
  • The Parallel Pain
  • Put the Pieces in Place for SERDES Success
  • Know your limits
  • November 2011
  • Shorter stubs are getting longer
  • Stupid vias… {grumble grumble}
  • Via modeling – what do I really need?
  • August 2011
  • HyperLynx PI Virtual Labs Launch!
  • Measurement correlation is just a stackup away
  • Your traces aren’t square, but do you need to care?
  • Can you make Z higher?
  • May 2011
  • Try to fit some plane pairs in your stackup
  • High impedance drives your stackup geometries
  • Stackups: More than just a bunch of routing layers
  • March 2011
  • Ever wonder the effects of shared anti-pads on differential signals?
  • January 2011
  • The length of your terminator doesn’t matter
  • Vias are longer than their length
  • How do you manage your trace lengths?
  • S-parameters are for more than just packages
  • Making SERDES sims faster with IBIS-AMI
  • Tired of waiting for your SPICE to finish?
  • October 2010
  • What’s driving the need for PCB power design?
  • July 2010
  • HyperLynx 8.1 released!
  • June 2010
  • Fundamentals of SI (Part 3) – Impedance
  • May 2010
  • Fundamentals of SI (Part 2) – Transmission lines
  • April 2010
  • Going from rules of thumb to simulation
  • Fundamentals of SI (Part 1) – Critical nets
  • Fundamentals of Signal Integrity
  • March 2010
  • Do you want to be a professional?
  • February 2010
  • The kindred spirit of an Olympian
  • A great start to DesignCon
  • January 2010
  • DesignCon 2010 – Next week
  • AMI – The next modeling frontier
  • DesignCon Baby!
  • December 2009
  • What’s your excuse?
  • Santa’s helpers – The empoverished life of an engineer
  • November 2009
  • HyperLynx DDRx Wizard Resources
  • A Late Night in Copenhagen
  • October 2009
  • The Halloween Rush