Ublox LISA-U2 Series, System Integration Manual

Page: 121 / 183

LISA-U2 series - System integration manual
UBX-13001118 - R27 Design-In Page 121 of 183
C1-Public
2.2.1.1 RF antenna connection
The ANT pin (main RF input/output) and the ANT_DIV pin (RF input for diversity receiver provided by
LISA-U230 modules) are very critical in layout design.
Proper transition between ANT and ANT_DIV pads and the application board must be provided,
implementing the following design-in guidelines for the layout of the application PCB close to the ANT
and ANT_DIV pads:
•
On a multi layer board, the whole layer stack below the RF connection should be free of digital lines
• Increase GND keep-out (i.e. clearance) for ANT and ANT_DIV pads to at least 250 µm up to
adjacent pads metal definition and up to 500 µm on the area below the module, as described in
Figure 56
• Add GND keep-out (i.e. clearance) on buried metal layers below ANT and ANT_DIV pads and below
any other pad of component present on the RF line, if top-layer to buried layer dielectric thickness
is below 200 µm, to reduce parasitic capacitance to ground (see
Figure 56 for the description of
the GND keep-out area below ANT and ANT_DIV pads)
Min. 500
µ
m
Min.
250 um
Top layer Buried metal layer
GND
plane
Microstrip
50 ohm
Figure 56: GND keep-out area on top layer around ANT and ANT_DIV pads and on buried layer below ANT and ANT_DIV pads
The transmission line from the ANT pad and the ANT_DIV pad up to antenna connector(s) or up to
the internal antenna(s) pad must be designed so that the characteristic impedance is as close as
possible to 50
 .
• The transmission line up to antenna connector or pad may be a microstrip (consists of a
conducting strip separated from a ground plane by a dielectric material) or a strip line (consists of
a flat strip of metal which is sandwiched between two parallel ground planes within a dielectric
material). In any case must be designed to achieve 50
Ω
characteristic impedance
• Microstrip lines are usually easier to implement and the reduced number of layer transitions up to
antenna connector simplifies the design and diminishes reflection losses. However, the
electromagnetic field extends to the free air interface above the stripline and may interact with
other circuitry
• Buried striplines exhibit better shielding to external and internally generated interferences. They
are therefore preferred for sensitive application. In case a stripline is implemented, carefully check
that the via pad-stack does not couple with other signals on the crossed and adjacent layers
Figure 57 and Figure 58 provide two examples of proper 50

coplanar waveguide designs. The first
transmission line can be implemented in case of 4-layer PCB stack-up herein described, the second
transmission line can be implemented in case of 2-layer PCB stack-up herein described.