Tip / Sign in to post questions, reply, level up, and achieve exciting badges. Know more

cross mob

EZ-USB™ FX3: Open-source, KiCad-based schematic and layout for FX3 camera kit - KBA236085

lock attach
Attachments are accessible only for community members.

EZ-USB™ FX3: Open-source, KiCad-based schematic and layout for FX3 camera kit - KBA236085

Infineon_Team
Employee
Employee
50 replies posted 25 likes received 25 replies posted
Version: *A
 

This KBA provides the schematic design capture and layout of the DEMO_FX3_U3V_CAM01 EZ-USB™ FX3 camera kit in KiCad. The FX3 symbol file and FX3 camera kit schematic, BOM, netlist, FX3 footprint and layout file are attached with this KBA.

KiCad is a free electronic design automation (EDA) software that facilitates the design and simulation of electronic hardware. It features an integrated environment for schematic capture, PCB layout, manufacturing file viewing, SPICE simulation, and engineering calculation.

1 Getting started


1. See Getting started with KiCad for basic information on how to use KiCad for schematic capture.

2. Download the DEMO_FX3_U3V_CAM01 FX3 Camera Kit Base Board.zip file attached with this KBA and extract it to a local folder in your PC.

Once extracted, the following files are available as shown in Figure 1:

File name

Type

DEMO_FX3_U3V_CAM01 FX3 CAMERA KIT Base Board Layout.kicad_pcb

Layout

DEMO_FX3_U3V_CAM01 FX3 CAMERA KIT Base Board Schematic.pdf

Schematic

DEMO_FX3_U3V_CAM01 FX3 CAMERA KIT Base Board Project.zip

KiCad Project file archive

DEMO_FX3_U3V_CAM01 FX3 CAMERA KIT Base Board BOM.xls

BOM

FX3 Symbol.zip

FX3 symbol file

FX3 Footprint.zip

FX3 footprint file


Infineon_Team_0-1687428098931.png

Figure 1  Extracted folder

3. Extract the project archive (DEMO_FX3_U3V_CAM01 FX3 CAMERA KIT Base Board Project.zip) to a local folder on your PC.

4. Use the KiCad application to open the KiCad schematic project file (DEMO_FX3_U3V_CAM01 FX3 CAMERA KIT BASE BOARD.kicad_pro) from the extracted folder.

2. DEMO_FX3_U3V_CAM01 schematic design


2.1 Creating EZ-USB™ FX3 design


1. Extract the FX3 Symbol.zip file.

2. Copy the FX3 symbol file (FX3 USB3.0.kicad_sym) from the extracted folder and paste it in the symbol’s library directory (kicad/library/symbols) as shown in Figure 2.

Infineon_Team_1-1687428224034.png

Figure 2  KiCad symbol library directory

3. After adding the FX3 symbol file in the library directory, click Add a symbol in KiCad application (see 1 in the below image) and add the CYUSB3014-BZXI device symbol into the schematic as shown in Figure 3.

IFX_Community_2-1663668042272.pngFigure 3  Adding symbol in the schematic from the library
 
Note:  By default, the number of units per package is 1, which indicates a homogenous component. Heterogenous parts will have more than one number of units per package. See FX3 Symbol file for all units of the CYUSB3014-BZXI symbol. Note that the units are visible only when the symbol is called in the project.

4.Similarly, create symbols of all the components used in the design in their respective directories inside the library.

2.2 View the schematic


Figure 4
shows a portion of the FX3 camera kit schematic using KiCad. Open the FX3 Camera kit schematic file using the KiCAD application to view the complete file.

IFX_Community_3-1663668267463.png

 

Figure 4  Schematic diagram of FX3 USB TYPE-C connector interface

As shown in Figure 5, every component in the schematic should have symbol properties so that all components properties are added to the Bill of Material (BOM).

IFX_Community_4-1663668301072.pngFigure 5  Symbol properties of FX3 symbol

2.3  Electrical Rule Check (ERC)


1. Annotate the entire schematic before performing ERC as shown in Figure 6.

IFX_Community_0-1663668882039.pngFigure 6  Annotation of schematic drawing

2. Perform ERC to check for errors and warnings in the design as shown in Figure 7.

IFX_Community_1-1663668957541.pngFigure 7  Performing electrical rules checker

Note : Make sure that all the warnings and errors are resolved.

2.4  Generating the Bill of Materials (BOM)


1. Click Tools and select Generate BOM as shown in
Figure 8.

IFX_Community_2-1663669084173.pngFigure 8 Generating the BOM

2. Select the appropriate script from the list to generate the BOM as shown in Figure 9.

IFX_Community_3-1663669168825.pngFigure 9 BOM generator script with specified location

3. Navigate to the local directory (#2 in Figure 9 refers to the local directory where BOM is extracted) and open the CSV file in Microsoft Excel as shown in Figure 10.

IFX_Community_4-1663669248604.pngFigure 10 BOM .csv file location

4. Edit the BOM as appropriate as shown in Figure 11.

IFX_Community_5-1663669309080.pngFigure 11  BOM Excel sheet

2.5 Generating the netlist


1. Click File > Export > Netlist as shown in Figure 12.

IFX_Community_6-1663669386592.pngFigure 12  Creating Netlist

2. Select KiCad and click Export Netlist as shown in Figure 13.

IFX_Community_7-1663669438909.pngFigure 13  Exporting the netlist

3. Specify your preferred location as shown in Figure 14.

IFX_Community_8-1663669507693.pngFigure 14  File location of netlist

4. Check the connections from the netlist against the schematic as shown in Figure 15.

IFX_Community_9-1663669568190.pngFigure 15  Netlist viewer

Note:  KiCad can be used to design PCB layout as well.

3 DEMO_FX3_U3V_CAM01 PCB layout


3.1 Creating the EZ-USB™ FX3 footprint


1. Extract the FX3 Footprint.zip file.

2. Copy the FX3 footprint file (CYUSB3014-BZXC.kicad_mod) from the extracted folder and paste it in the local footprint library directory (kicad/projects/FX3 Camera Kit/My_Footprint.pretty) as shown in Figure 16.

Infineon_Team_2-1687428962565.pngFigure 16 Adding the FX3 footprint file in the footprint directory

3. After adding the FX3 footprint file in the footprint directory, double-click the symbol in the KiCad Schematic Editor application and select the CYUSB3014-BZXI footprint from the footprint directory, as shown in Figure 17.

Infineon_Team_3-1687429030401.pngFigure 17 Linking the footprint in the schematic from the directory

4. Similarly, link the footprints of all the components used in the design to their respective directories inside the footprint library.

3.2 Layout view


Figure 18
shows a portion of the FX3 camera kit layout using the KiCad PCB Editor application.

1. Open the FX3 camera kit PCB file (DEMO_FX3_U3V_CAM01 FX3 CAMERA KIT Base Board Layout.kicad_pcb) using the KiCad application to view the complete file.

Infineon_Team_4-1687429120371.pngFigure 18 TOP layer PCB viewer

2. As shown in Figure 19, switch ON and OFF all the layers as per the requirement.

Infineon_Team_5-1687429164653.png

Figure 19 All layers viewing stack up

3.3 Design Rule Check (DRC)

 


1. As shown in Figure 20, perform DRC to check for errors and warnings in the layout.

Infineon_Team_6-1687429254816.pngFigure 20 Design Rule Check

Note: Make sure that all the warnings and errors are resolved.

3.4 Silkscreen clean-up


1. Perform the silkscreen clean-up on both the layers (top and bottom) and add the company logo and RoHS details as per the requirements for a better understanding, as shown in Figure 21.

Infineon_Team_7-1687429350194.pngFigure 21 Silk clean-up

3.5 Fabrication notes


1. Write the fabrication notes for the manufacturer and add the drill table, board characteristics, board size, and stack-up table in detail1 and detail2 layers, as shown in Figure 22.

Infineon_Team_8-1687429416818.pngFigure 22 Fabrication notes

3.6 Generating Gerber


1. Go to File, click Fabrication Outputs, and select Gerber to generate the final Gerber (file/fabrication outputs/gerbers) for the manufacturing as shown in Figure 23.

Infineon_Team_9-1687429481595.pngFigure 23 Generating Gerber

2. Select Plot format as Gerber, browse the output directory, and select fabrication layers (top, bottom, gnd1, gnd2, pwr1, pwr2, signal1, signal2, silkscreen, front and bottom mask, detail1 and detail2) as shown in Figure 24.

Infineon_Team_10-1687429523605.png

Figure 24 Fabrication layers

3. Go to File, click Fabrication Outputs, and select Drill Files. Add the drill file to the Gerber as shown in Figure 25.

Infineon_Team_11-1687429583118.png

Figure 25 Fabrication layers

4. Go to File and click Fabrication Outputs, select IPC-D-356 Netlist File, browse the Gerber directory, and add the netlist file to the Gerber as shown in Figure 26.

Infineon_Team_12-1687429641007.png

Figure 26 Fabrication layers

Attachments
1299 Views