Design & Order Customized FPC Cable Using KiCAD

This guide is for designing a customized 2 layer FPC cable that can go in a 40 pin, 0.5mm pitch Zip connector optionally will show how to do impedance controlled traces in FPC. It's fairly easy to design one and order in a PCB house like PCBWay.

FPC a circuit that printed in a flexible sheet. For more details checkout this post. FPC and FFC is not same type of cable. FPC can have Impedance controled traces, custom design, multiapl layers which are lacking in FFC.

Please watch the guide for more details and the video have chapters for quick navigation.

Reference FPC connector

This FPC will be used to connect 2 PCB that has both high and low speed traces. So existing connector will be used to connect this FPC to the PCB. A 40 pin, 0.5mm pitch connector from Würth Elektronik will be used.

• https://www.digikey.no/en/products/detail/w%C3%BCrth-elektronik/687140149022/5047804

Reference FPC Cable

And to a reference design of a cable that fits into that connector will be helpful to design the FPC easier. Again a FFC cable from Würth Elektronik will be the reference.

• https://www.we-online.com/components/products/datasheet/687640100002.pdf

First the connector that goes into the zip connector is made as a footprint, that way it can be reused on both side. This is done in these steps

Create Footprint: From the KiCAD's Footprint Editor press "File" >> "Create footprint" and give it a name.

Add Pad: Start by selecting the "Add Pad" tool, ensure that you set the dimensions accurately based on the specifications provided in the reference datasheet for the connector, which is Cw=0.3mm and S1=4mm.

Replicate Pads: Once you've created the initial pad, replicate it to produce a total of 40 pads. You can do this by selecting the pad and then right-clicking. From the context menu, choose "Create from Selection" >> "Create Array." Specify the number of "Horizontal count"=1, "Vertical count"=40, "Vertical spacing & offset" =0.5(same as FPC pitch), "Stager"=1 and others set to 0. Then click "OK" to generate the array.

Center Alignment: After creating the array of pads, select all the pads and move them to the center along the axis to maintain symmetry and alignment.

Draw Edge Cut line: Switch to the "Edge Cut layer" by selecting it from the right side menu. Create a straight line that matches the width of the FPC cable that will be connected to the connector, which is W=20.5mm in the reference datasheet.

Save the Footprint: Once you've completed the design of the connector footprint, save it.

Add Symbol: Open the schematics editor and locate the "Add a symbol" option in the toolbar on the right side. Use this tool to search for a symbol with the same pin count as the FPC, which is 40 for this design. Once you find the suitable symbol, place it onto the schematic sheet.

Assign Footprint: Double-click on the symbol you just added to open its properties. Look for the option "Footprint" and press the library button on the end. Select the footprint that was created in the previous step from the available options.

Duplicate Symbol: Create a duplicate of this symbol to represent the other side of the connector. You can do this by selecting the symbol and using the good old copy/paste.

Ground Lines: Ensure that there are an adequate number of ground lines in the connector symbol. This is crucial for impedance-controlled traces. Having sufficient ground lines allows for a reference for the layer opposite to the signal traces in the FPC. This ensures proper grounding and minimizes signal interference.

Connect Pins: Now connect both connector symbol pins to each other one by one and save.

Pull Schematic Changes: Open the PCB Editor and pull the changes from the schematic using the button "Update PCB with changes made in the schamatics" located on the top toolbar. This should automatically place two footprints on the PCB editor corresponding to the connectors added in the schematic.

Place Connectors: Position both connector footprints on the PCB editor facing opposite to each other. Ensure that the distance between the edge cuts of both connectors matches the length of the FPC cable, which in this design is 27mm.

Create PCB Outline: Switch to the "Edge Cut layer" by selecting it from the right side menu. Use the "Draw a line" tool available in the toolbar on the right side, draw lines to connect the edge cuts of both connector footprints. Ensure that the lines form a closed shape, outlining the perimeter of the PCB. This closed shape defines the physical size of the cable.

PCB House like PCBWay needs a reference of the size and the position of the stiffener to get them manufacture it correctly.

Select Layer: Open your PCB design software and select the "B.Silkscreen" layer from the right-side panel. This layer is suitable for indicating the position and size of the stiffener as it will be placed on top of the B.Cu layer.

Draw Stiffener Outline: Use the "Draw a Rectangle" tool from the right-side toolbar to draw the outline of the stiffener on the "B.Silkscreen" layer. Manually set the size of the rectangle by double-clicking on the outline, that is 20.5mm and 8mm.

Add Dimension: Utilize the "Add an aligned linear dimension" tool from the right-side toolbar to create dimensions for the stiffener outline. This provides precise measurements that the PCB manufacturer can use to accurately position and size the stiffener during fabrication.

Add Text Label: Use the "Text" tool from the right-side toolbar to add a text label beside both the stiffener outline and the dimension lines. Label the text as "Stiffener" to clearly indicate its purpose and help the manufacturer identify it easily.

Connect the pins usually using the route trace tool from the right side tool bar. Select the trace width according to your needs.

Don't connect the Ground traces if there are impedance controlled traces. Because ground needs to be transfer to the other layers using vias. So keep them unconnected if there are impedance controlled traces.

Will do some traces with 100ohm impedance.

Know the PCB House Capabilities: Look for capabilities of the PCB fabrication house, this includes their minimum trace width, minimum spacing, and any other design constraints they may have. For PCBWay they can do ≥0.06mm trace and spacing. And spacing between the layers (or FPC thickness) are 0.1mm is selected for the 100hom traces.

Access the Board Setup Tool: Open "Board Setup" tool from top tool bar. This tool allows you to define design rules, including net classes for different types of traces.

Define Net Classes: Within the "Board Setup" tool, navigate to the section for defining net classes. Here, you can create net classes for different types of signals, such as single-ended traces, differential pairs, power traces, etc.

Set Trace Sizes and Widths: When setting up net classes for differential pairs, ensure that you specify the correct trace width and spacing required for differential signaling. This can be calculated using the "Calculator tool" of KiCad. For this design 0.08mm width, 0.06mm spacing trace is used for differential traces used in the this design.

Assign the traces: In the "Schematics Editor" select the pair of traces that need to be the differential traces, name those trace 1N/2P using the "Add a Net Label" tool from the right side toolbar. Then right click select "Assign Netclass.." and select the net class just being made in the 2nd step.

Basically one need to follow the PCB house capabilities to set the trace size and width of the differential pairs and setup this the the Board setup tool >> Net Classes

Access the Add Field Zone Tool: Locate and select the "Add Field Zone" tool from the toolbar on the right side of the interface. A popup window will appear, choose the GND NET from the list of available nets.

Choose Copper Layers: In the left side menu of the popup window, ensure that both the F.Cu (Front Copper) and B.Cu (Back Copper) layers are selected. This indicates that the copper zone will be applied to both sides of the FPC. Now draw the zone area, make sure the area is out of the FOC outline area.

Fill the Zone: Once you've drawn the outline of the copper zone, press the "B" key on your keyboard to fill the zone. This action fills the outlined area with copper on both the front and back layers of the FPC. Whenever there is a change in the FPC, refill the zone using the "B" key. This ensures that the copper layers are always up to date with the latest design changes.

Via Size: Vias can be smaller in Flat Flex PCBs, set the via size accordingly. For this design, used a 0.15mm hole size with a 0.30mm outer copper line, aligning with PCBWay's capabilities.

Connect Ground Traces: Place vias along the Ground traces to establish connections between the ground traces coming from the connector and the ground plane. While placing the traces press "V" to place the via. Ensure that the via size matches the specified dimensions (0.15mm hole size and 0.30mm outer copper line).

Rebuild Copper Zone: After adding vias, rebuild the copper zones on both sides of the Flat Flex PCB layout by pressing the "B" key.

Generating the Gerber is same as regular PCB.

Selecting folder: Select File >> Fabrication Outputs >> Gerbers. Select a folder that is in the project folder, else the files will be created on the projects folders where other files are.

Build the drill files: Generate the drill files first by clicking the button on the bottom of the window. Then close that drill files window and press plot button on the bottom of the window.

Zip it: Now all the files are generated and placed inside the selected folder. Now create a zip of that folder.

As I am ordering my board from the PCBWay, so this part is presented using thier website.

Website: Go to their website PCBWay.com and select PCB Instant Quote option and select the FPC/ Rigid-Flex. Or click this direct link .

Configure PCB Parameters: Specify the following parameters:

• PCB Type: Flexible PCB
• Different Designs in Panel: 1 (this is only single design)
• Layer: 2 (as this desing have 2 coper layers)
• Base Material: Polyimide Flex
• FPC Thickness: 0.1mm (according to our impedance controlled trace requriments)
• Stiffener: Select BOT >> BOT PI >> (0.2mm)

Other Opions: Keep other options as default, some options like, "Surface finish", "Solder mask", "Silkscreen" etc are not that important for this design requriment. Go change them if you want more customizations.

Calculate Quote: Press calculate and later it will ask for the gerber file, then upload the zip that is created on previous step.

Last step: Now PCBWay engineer will look at the desing and approve the order than you can do the payment. you will get the finished