here - Case IEEE - Case Western Reserve University

Using Eagle for
PCB design
Part 2, high speed mixed
signal design techniques
Mike Twieg
Case Western Reserve University
November 21st 2011
• Wrap up from part 1: Exporting design files from Eagle, and
submitting files for manufacturing
• Recommendations on SMT packages
• High speed signal propagation
• Mixed signal layout design
• 4 layer design techniques
Design finishing checklist
• Make sure the design rule checker (DRC) settings match the
design for manufacture (DFM) rules for the manufacturer
• No DRC errors (unless you are sure they are benign)
• No outstanding ERC warnings. No design inconsistencies
• No unrouted traces
– Turn off all layers except “unrouted,” you should see nothing
• If you intend to have a silkscreen printed:
– You can export any layers to the silkscreen during the CAM process
– Common layers: Names, values, place, docu
Gerber files
Gerber is a common CAD format which describes images using
Industry standard is now RS-274X (extended Gerber format)
Several Gerber files are needed, each having info from multiple
layers in your layout editor
Information on drill hits is not included in Gerber files.
Excellon files contain drill coordinates and sizes.
The CAM processor
The CAM processor is used to export the Gerber and Excellon files
Open the CAM processor through the layout toolbar
The CAM uses job files to perform specific tasks
• Export Gerber files with
• Export Excellon drill file with
Exporting Gerber files
Each tab is a different Gerber file
to be generated
We highlight which layers in the
layout editor are exported to
each Gerber file
Eagle does most of the work for us
For two layer designs, we should
only need to choose which
layers to export to the
silkscreen(s). Usually
dimension, place, value, and/or
docu layers.
Make sure all the layers you want to export are enabled in the layout editor!!
Exporting Excellon drill file
Now open up the job
Exporting the Excellon file is even
easier than the Gerber files
Use default options, unless you
really know what you are
Make sure all the layers you want to export are enabled in the layout editor!!
Preparing design files
After running the gerb274x and excellon job files, you should
end up with up to 9 files total with the following extensions
Filename.cmp (top copper layer)
Filename.sol (bottom copper layer) (top soldermask layer)
Filename.sts (bottomsoldermask layer)
Filename.plc (top silkscreen layer)
Filename.pls (bottom silkscreen layer)
Filename.drd (excellon drill file)
Filename.dri (info on drill toolset – not needed)
Filename.gpi (general board info – not needed)
Rename each file with its specific function, and put them all in
one ZIP archive
Previewing Gerber files
If you want to examine your Gerber files, you can use Pentalogix Viewmate.
The free version allows you to easily view, but not edit, gerber files.
Hint: if your drill data looks “exploded” when imported, check the settings on leading/trailing zeros
Submitting files for fabrication
The steps for submitting files will depend heavily on the
It is highly recommended that you first use the manufacturer’s
DFM (Design for Manufacturing) checker to check that your
design conforms to their capabilities
If you don’t pass their DFM checker, then you must change your
DRC rules to be consistent
We will be using Advanced Circuits as an example
Using Advanced Circuits
First use the DFM checker at
• When submitting the files for a DFM check, you will upload the zip file
with your design
• You must tell the DFM checker which file corresponds to which layer or
• You must also tell it some specifications of the design (number or layers,
size, etc)
• Submit the files and wait for results via email…
If you pass the DFM checker, you may then submit the design for
The process for ordering boards is almost identical to using the
DFM checker, plus shipping and billing information
Advanced circuits free DFM checker
Advanced circuits DFM checker
Using the DFM checker
After submitting, you should receive an automated analysis from, which includes two things of importance:
• Plots layer review, which shows you PDF images of each layer
• Any DFM errors found. All “show stoppers” should be fixed. Potential
problems can often be left alone (especially ones relating to silkscreen
If you pass the DFM check, then
you can order the board for
real. The process for ordering is
almost exactly the same as for
the DFM check.
Leaded IC packages
1.27mm (easy)
0.65mm (medium)
0.5mm (difficult)
Leaded IC packages
0.5-0.65mm (not too bad)
0.4-0.5mm (pretty hard)
Many varieties
BGA (death is certain)
Two terminal packages
For resistors/capacitors and inductors, 0805 is a good
compromise between difficulty and density:
For diodes, SOD123 and SOD323 are good choices:
Often larger packages are needed in order to dissipate enough
power or store more energy. Pay attention to component
High speed layout techniques
Special care must be taken when designing PCBs for high speed
digital communication and analog systems
These techniques apply well to signals in the regime where
transmission line effects are still negligible
• 50mbps for digital data signals, 100MHz for analog
• Remember, digital signals have bandwidths far above their baud rates!
• Normally care about up to 5th-7th harmonics for data signals, 7th-9th
harmonics for clock signals!
First we look at how to preserve intentional signals
High speed signal propagation
All high speed signals should be adjacent to at least one reference plane
At high frequencies, currents in traces will return in any adjacent planes
Cross section of microstrip trace
Cross section of stripline trace
Return current paths
Example: one microstrip trace with a source and a load
Z  L A
Return current paths
At high frequencies, return currents want to form smallest loops
Therefore they try to run underneath the signal traces
Current distributions for high speed microstrip trace
Return current paths
Return currents can be interrupted by split reference planes
These large current loops will cause distortion and emit additional EMI!
Bypass capacitors
Bypass capacitors are critical for keeping low loop areas and low
impedances at high frequencies
Bypass capacitor selection
For bypass caps to be effective:
• Should be placed as close to the IC supply pins as possible
• Use at least one per IC
Capacitors are not perfect: self resonance
• Can deal with self resonance by using
several capacitors in parallel of
different sizes
• Smaller packages will have lower ESL,
higher SRF
Stitching capacitors
Can bridge plane splits with capacitors, allowing return currents to pass
This will reduce isolation between the two planes at HF. This is not wise,
especially when crossing to or from analog partitions!
Signals changing layers
Sometimes it is necessary to have a signal change layers with a via
When this is done, the return current also changes layers!
Need to provide a good path for the return current between layers
• Use vias to locally connect the two
• This only works when those two
planes are actually the same
Signals changing layers
When changing layers AND changing reference planes, we cannot use a via for
return currents
This is often the case with 4 layer board stackups (signal, GND, Vs, signal)
We can use stitching caps to improve return currents
Even so, this is a mess and is not suitable for very high speeds…
Simply put, high speed signals should not change reference planes!
Differential signaling
Differential signals use pairs of traces to form closed current loops
Return currents on reference planes are greatly reduced
Pairs must be routed close together to be effective
Not a perfect solution: can still carry common mode return currents. Not the
same as signal isolation!
When all else fails…
If EMC/crosstalk performance is critical, then complete isolation may be
necessary to cross splits
Isolation can be optical or galvanic
Basic optocoupler
Digital magnetic coupler
Always some propagation delay, and limited bandwidth
Large packages, costly
Can be used for logic level translation
Very useful for interfacing to I/O ports where isolation is important
Mixed signal design
Mixed signal design: any design where analog and digital systems
operate in the same environment
If you have a DAC or ADC in your design, it’s mixed signal.
Power supplies may be considered analog systems
Good mixed signal design is critical when digital and analog
portions work at overlapping bandwidths
Mixed signal design goals
Our goal is to prevent unintentional signals form causing
interaction between digital and analog systems
Interaction can be caused by conduction and field coupling
Most basic rule is to spatially partition analog and digital sections
Design example: ADS8329 16 bit ADC
3.3V digital supply
5.0V analog supply
25MHz SPI interface
External analog shunt reference voltage
Use 9 pin header for digital signals and power supplies
Use edge SMC connector for analog signal in
Example schematic
Example Layout
Example Layout
All high speed
signals have
their own
return paths
Ferrite bead
across split
Reference is
grounded on
analog side
Bypass caps
close to supply
Example Layout (bottom layer only
We can make multiple sub-partitions by making additional splits
in the reference planes
This can decrease crosstalk between analog channels
We do not split the ground plane completely
The analog and digital supply pins of ADCs/DACs must be kept close to the
same potential
Common practice is to join the supply planes only underneath the ADCs/DACs
Signal traces may only cross between partitions at that point
Q: Do we need completely different power supplies for different partitions?
A: No, but we need to partition that power supply using split planes, ferrite
beads, and bypass capacitors so that the two partitions do not share
current paths at HF
Choking supplies
Example: Using one regulator for both digital and analog partitions
A ferrite bead provides HF current loops between the two partitions
Ferrite beads
Capacitors are useful for encouraging HF current to flow along certain paths
Ferrite beads are high impedances at HF, and prevent HF currents from
flowing through them
Ferrite beads are not inductors
Both imaginary and real
impedance increase with
frequency, peak, and then
Forms damped resonances
with bypass capacitors, so
much less ringing
Considerations for SMPS
Switch mode power supplies present great challenge
Generate high dv/dt and di/dt, which causes lots of emissions
Prevent B field emissions by minimizing loop areas
Prevent E field coupling by screening with reference planes
Considerations for SMPS
Switch mode power supplies present great challenge
Generate high dv/dt and di/dt, which causes lots of emissions
Prevent B field emissions by minimizing loop areas
Prevent E field coupling by screening with reference planes
Very high
Considerations for SMPS
Switch mode power supplies present great challenge
Generate high dv/dt and di/dt, which causes lots of emissions
Prevent B field emissions by minimizing loop areas
Prevent E field coupling by screening with reference planes
Very high
Very high
Considerations for SMPS
High di/dt loop is minimized
Capacitive coupling from
high dv/dt node may be an
• Can use ground layer as a
screen by putting other
sensitive components on
bottom side
• Always best to move
SMPS as far from analog
circuitry as possible
Beyond two layers
When it is not possible to adhere to good design techniques, you may need
more layers
Common four layer stackup:
• One inner layer is for ground
plane(s) only.
• Other inner layer is reserved
for non-ground supply rails
• Outer layers are for traces and
Spacing between each layer may not be equal! Very important for high
speed design.
Distributed capacitance between inner reference layers is useful for high
frequency bypassing
Four layers
Four layer designs have two key advantages
• Separate layer for power supply routing
• Both sides are freely available for components and signal traces
This allows for much easier design and higher density
However, in general, signals
cannot change layers in this
stackup without changing
reference planes
Properly guiding return currents
across multiple reference planes
is difficult
Therefore, unless you do not
need signals to change layers,
four layer designs are not
suitable for high frequency
Six layers
One common six layer stackup: equivalent to four layer stackup with two
more outer signal layers added
Signal layers 1 and 2 both use reference layer 3 for return
Signal layers 5 and 6 both use reference layer 4 for return
Traces on layer 1/6 run orthogonal to traces on layer 2/5, to reduce crosstalk
Six layers
Another six layer stackup: equivalent to four layer stackup with two more
inner signal layers added
Signal layers 1 and 3 both use reference layer 3 for return
Signal layers 4 and 6 both use reference layer 5 for return
Traces on layers 3 and 4 should run orthogonal to prevent crosstalk
Effective high layout design is all about controlling current paths
• Intended current paths should be uninterrupted and low impedance
• Unintended current paths should be minimized with proper partitioning
and isolation
Number of layers and stackup type will depend on design
• It is perfectly reasonable to have very high bandwidth systems on 2 layer
boards. However, traces cannot cross or change layers easily
• Moving to four layers allows more freedom for routing traces, on both
sides, but traces still cannot change layers without risking signal integrity
• In complex designs in which signal busses must cross, at least six layers will
usually be necessary
Proper mixed signal design is achieved by preventing shared
current paths between analog and digital systems
• Component placement is at least as important as signal routing
• We do not use completely split ground planes, but rather partitioned
planes which connect at specific locations
• Multiple sub-partitions can be made by further dividing the reference
• Analog and digital partitions can share supply rails, but care must be taken
to introduce new high frequency current paths
Any questions?

similar documents