Fundamentals of SI (Part 3) – Impedance

We’re finally on to the next logical step in our study of signal integrity – impedance.  So what is impedance and why does it matter?

Impedance is a result of the physical properties that make up your PCB and the reason you care about this is because the impedance of your traces will have an impact on the signal quality.   If you remember from Part 2 of this series on transmission lines, I talked about critical length.  Well, one important aspect of transmission lines left out of that topic (on purpose) was that once t-lines are beyond the critical length, the impedance becomes important because it can cause reflections and distort signal quality.  Matching impedance for driver, transmission line, and receiver becomes important to ensure you’ve got good signals at the receivers.  Reflections are a topic in-and-of themselves, so I’ll reserve that for a future post, but below is what you need to know about transmission line impedance.

The basic formula for characteristic impedance is:

Characteristic Impedance

Characteristic Impedance

We can see that it’s made up of the capacitive and inductive properties of the trace.  So what does this mean to a board designer? You can impact what the impedance of your traces are, largely based on your stackup design.  Here are the main things in the stackup that we can use to control the impedance: dielectric thickness, dielectric constant, and trace width.  The copper thickness can also play a part but it is less significant.

With dielectric thickness, we’re trying to determine how far away the trace should be placed from it’s reference layer(s).  This is often ground for ideal situations but it could be a power layer as well.

Stripline and Microstrip structures

Stripline and Microstrip structures

We also need to consider that the trace could be a microstrip (on the outer layer of the board) or a stripline (on an inner layer with references above and below the trace) structure.  There are other types of structures such as dual stripline or buried microstrip but I just wanted to provide an example of 2 of the primary types of structures you’ll deal with.   In both examples, when you decrease the dielectric thickness, you’ll decrease the impedance.  Likewise, increasing thickness will increase impedance.  Generally speaking, for the same dielectric thickness and trace width, you’ll have a higher impedance on a microstrip line than you will for a stripline because of the additional capacitance provided in the stripline structure.

The other important piece relative to the dielectric is the dielectric constant.  Standard FR4 material in most PCBs will have a relative dielectric constant (commonly seen as Er or Dk – these symbols are interchangeable) on average of about 4.3 but if you choose a dielectric with a much lower Er, it will cause the impedance to increase.  Similarly, if you were to increase the Er, it would cause the impedance to go down.  The leaver you have to control the Er is the laminate you choose for the stackup design.  If you want to see your options in more exotic materials, check out Isola or Rogers who are just two options of several in the laminate material industry.

The last factor that can play a major part in trace impedance is the trace width.  If you increase the trace width, the impedance will go down.  If you decrease the width, the impedance will go up.

So what makes all these properties behave the way they do?  You can trace most of the changes down to how the capacitance is calculated. Looking at the equation for capacitance in a parallel plate, we can see there is dependency on dielectric constant, separation between the plates (d), as well as the area (A).

Capacitance

Capacitance of parallel plate

We can see that if the Er changes, that has a direct relationship on the capacitance.  And going back to the characteristic impedance equation, it has an inverse relationship on impedance (e.g. Er goes up → impedance goes down).  We can also see that as the separation between the two parallel plates increases, it has an inverse relationship on the capacitance, which means it has a direct relationship with the impedance (e.g. separation goes up → capacitance goes down → impedance goes up).   And lastly, the area changes based on the trace width, so if the trace width goes up, capacitance goes up, which means the impedance goes down.

There are stackup planning tools in HyperLynx as well as Expedition which can simplify your life when it comes to impedance planning.  It can be as simple as entering a target impedance for a layer given a certain stackup and HyperLynx will tell you the the trace width you need.  Or you can enter a width and it will give you an impedance on any given layer.

stackup

I’ll leave you with some final thoughts on impedance control from a practical perspective.  For most companies, if you design impedance controlled boards, your manufacturer is going to adjust whatever values you give them to hit the target impedances based on the materials they have on-hand.  You may specify 6 mil width for traces and they may do 5.6 mils in production, but the end result that matters is that they are meeting your target impedance.  One trick to give your manufacturer more ability to hit impedance goals is to specify slight differences in trace width for your targeted impedances, especially when it comes to differential impedance (I haven’t even touch on differential impedance here so I’ll save that for another post ).  For instance, on Layer 4 of your stackup, you may have a 50 ohm target impedance which results in a 5 mil trace width for single ended traces, and a 100 ohm differential impedance with 5 mil traces on the same layer.  For the single ended traces, just put 5.1 mils into your design and for the differential, make it 4.9 mils.  That will allow them to target both impedances for you independent of each other without having to make compromises to either target impedance.

To learn more about impedance and stackup planning, check out Chapter 10 of the HyperLynx QuickTour.

Post Author

Posted June 29th, 2010, by

Post Tags

, , , ,

Post Comments

No 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

Add Your Comment

Archives

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