P9027LP-R-EVK Layout Guide
AN-933
Application Note
© 2016 Integrated Device Technology, Inc
1
May 16, 2016
Using the Reference Layout
The P9027LP-R-EVK reference layout is a full feature four-layer design optimized for high-performance, small-size, and ease-of-use. The
purpose is to minimize design-in effort and risk by providing a proven solution that can be imported into an existing system design. The
P9027LP-R-EV board layout can be divided into two parts; the main function layout (core layout) and the layout for test purpose. When
imported into an existing system, only the core layout is necessary. The core layout follows the design rules for wearable devices with
minimum space and trace width of 4 mils. The minimum finished VIA size is 4 mils, assuming 1 mil plating thickness. The minimum spacing
between components is 0.2 mm. Only through hole VIAs are used. There are no blind or buried VIAs. When circumstances permit, it is highly
recommended to copy the reference layout.
Importing the Reference Layout
The P9027LP-R-EVK reference design was created using Cadence PCB design software. This software has been used to generate the
layout modules, which can be rapidly deployed onto PCB designs, using Cadence, OrCAD, CIS and Cadence Allegro PCB Editor. The
P9027LP-R layout module is labeled P9027LP-R-EVK.mdd and may be loaded into an existing or new PCB design file by following these
instructions:
1. Use or copy the P9027LP-R-EVK schematic file (.dsn) and export the netlist to a PCB file.
2. Move the file P9027LP-R-EVK.mdd to the same directory as the PCB design file.
3. Import the netlist into the PCB file (.brd).
4. Open the PCB design file (.brd) and click on the menu PlaceQuickplace…
a. Select Place by Page Number and select the page the P9027LP-R circuitry resides on
b. Click Place. Click Ok..
Figure 1. Cadence Quickplace option box used for placing the IDT Layout module by Page Number.
5. Select the parts that were placed from the schematic that matches the schematic used from the P9027LP-R-EVK.
a. In the Find Filter, select Symbols, then left click and drag to highlight all of the components that were just placed.
b. Right click on any of the highlighted parts and select “Place Replicate ApplyBrowse…”.
c. Select the P9027LP-R-EVK.mdd file and select Ok.
d. Components should now be matched; if unmatched, manually identify and match component reference designators based
on schematic location.
6. Enter the coordinates(x,y location) in the command window where the P9027LP-R circuit should be located at, or left click where the
P9027LP-R should be placed.
© 2016 Integrated Device Technology, Inc
2
May 16, 2016
Connecting a Load
The reference board layout has been designed such that the DC output is easily accessible when being imported on to a system board.
Traces should be connected directly to the OUT and GND VIAs on the top or bottom layer, and routed to the load. Wide, low-impedance
traces are recommended to minimize the DC voltage drop on its way to and from the load. To reduce ripple voltages, or improve transient
performance, increase the capacitance on Vrect and OUT nodes.
Connecting Inputs / Outputs
All input and outputs on the reference board have been placed near the edges of the reference layout such that they can be easily connected
to other parts of the system board. After placing the module in the specific design, use the labeled VIAs as connection points for new traces
on either the top or bottom layer.
Manufacturing Notes
The PCB should be made with a minimum of 1oz copper foil weight per square foot or heavier.
Additional Resources
All support files and collateral for the P9027LP-R-EVK reference board can be found at www.IDT.com/WP3W-RK. Files include: schematics,
layout files, datasheets, user manual, etc.
Custom Layout Guidelines
The P9027L-R wireless power receiver is an integrated device consisting of multiple high-power blocks along with noise sensitive circuits all
controlled by a state-machine with some programmability. When designing the printed circuit board (PCB), there are multiple considerations,
and often some tradeoffs, associated with managing the critical current paths. In order to optimize the design, components should be placed
based on circuit function, to guarantee the best performance when the schematic is implemented in a PCB design. Furthermore the thermal
management of the application is important to the product’s performance and should be optimized during PCB design. By following the
guidelines set forth in this document, efficient operation will be obtained for each circuit function.
At the time that the layout is started the following guidance should be used to place the most critical parts in order of priority. There are three
main categories of circuitry: Power Circuits, Sensitive Circuits, and Non-Sensitive Circuits.