The best way to see the PCB layout is probably by downloading the KiCAD
project and exploring it. We will try here to give some explanations
using some screen captures.
To realise the layout, we use a 1,6 mm thick RF4 PCB, with 4 layers.
This printed board has a fabrication class of 5. (Desgin rules are 0.15
mm minimum track width and 0.24 mm for the minimum via
We have three parts that have to coexist on the board :
> # Analog part : very sensitive to noise
> # Digital part (including the MicroZed): generates a lot of noise
but has to be connected to the analog part at the ADC
> # The power supply : generates a lot of noise and takes a lot of
space on the board
According to the number of components and signals, we decided to use a
four layer board. The layers are organised following this order from the
top to the bottom :
> # components, analog and digital signals (in red on the picture
> # ground plane (in yellow),
> # power planes (in pink),
> # components and digital signals (in green)
Some consideration about ground splitting
A current always travels by performing a loop. A rule of thumb in
EMI/EMC is to keep the loops' area as small as possible. That is why we
put the ground plane on the second layer. By this way the ground current
will be close to the track on the surface of the board. Furthermore,
this layer acts as a shield and protects the analog signal on the top
layer from the noise generated by the digital tracks on the bottom
The power layer also acts as a shield between the top and bottom layers.
In addition, the planes have a lower impedance than any tracks and are
thus appropriate to transmit power.
Only one ground is used. Some books explain that it is necessary to
separate the analog and digital grounds when designing such a board
mixing both these signals. Indeed, it is possible that the fast digital
switching currents generate parasites on the analog components. In some
case, splitting the two grounds can be useless, or can give worse
results than without the separation. To understand that we first need to
understand how is spread the current in the ground plane.
If at low frequency, the current follows the path which has the lower
resistance, at high frequencies it follows the path of least impedance.
This path is on the ground plane, under the track itself. A rule of
thumb is that the return current in the ground plane will follow the
incoming current track when the frequency is above a few hundreds of
kilo Hertz. We have to pay attention at the ground plane state while
routing the different tracks.
For example, if we put a trace above the ground separation, the return
current would have no other choice than to follow the separation until
it arrives to the junction. This would not only increase the impedance
but would also increase the loop size (and thus its sensitivity to EMI).
If the tracks are correctly routed and the digital and analog parts
placed on different sides of the board, we do not have to separate the
two grounds as no digital ground currents would pass under the analog
The power supply part
We placed the power supply part on the right side of the board. The
presence of the buck converter constraints us to place it as far as
possible of the analog part. As the currents are relatively high in this
part of the schematic, we decided to link the components using planes
instead of tracks. On one hand this will lower the impedance and on the
other, these tracks will act as heatsink.
The MicroZed board has also been placed to have its own power supply as
far as possible of the analog components.
The buck converter works by cutting the current, which generates a lot
of electromagnetic parasites. The high current zone (between the buck
output and the coil) has to be small enough to not radiate.
Nevertheless, this zone can not be too small because it works as a
All the massive power components are placed on that side of the PCB. The
two LDO are placed next to the ADC. We then avoid a too long track and
As the ADC have many power inputs, we decided to use power planes
instead of making multiple tracks which would make the routing
difficult. These two planes are separated by the black lines on the
The analog part
There is a lot of decoupling capacitors next to the ADC. To be
effective, these capacitors have to be as close as possible of the chip.
The lowest capacitor value is placed on the first layer. Unfortunately,
as we do not have enough space to put all the capacitors on the same
side, we decided to put the others on the bottom
The main analog traces are on the top layer. For each channel, we put an
horizontal SMA connector on the border of the board and two vertical
connectors closer to the ADC. The first one is used to send a ground
referenced signal and the two others are used when the signal is
differential. The space between the two vertical connectors is 0,5 " to
be able to connect directly the LTC6954-1 Demo
Board which will be used to test
All the digital tracks going from the ADC to the MicroZed's FPGA have
the same length. The net lengths on the MicroZed board itself have been
compensated on the ADC board. For all differential tracks, we have a
differential impedance around 65 ohm at 100
All the differential signal (except these from the connectors) are delay
matched to better than 10 ps (3 mm on the board). The same has been done
for the clock splitter circuit : the ADC clock lines have the same
length. To avoid these lines to radiate some electromagnetic waves on
the analog traces, we route them on the bottom layer. The SMA is placed
as close as possible of the clock splitter to avoid the track to act as
The digital part
The connections to the MicroZed board are done to simplify the layout.
Using this configuration makes the connection tracks smaller and free of
vias. The same has been done for the connections to the connectors.