Slider

Example Slider Module for Jacdac, in KiCad

This is an example / reference Jacdac module for a slider potentiometer built in KiCad, an open-source PCB design suite.

Structure overview

This KiCad project uses local (per-project, relative path) references to the Jacdac symbol and footprint libraries that are included in this repository. This also includes a project-specific slider.pretty footprint library containing the module QR code, as generated by the Jacdac Silk QR Code generator.

Fabrication data (gerbers, pick-and-place) is included in the fab-1.1 folder.

Fabrication notes for JLC

We fabricated our prototype run for this board with JLCPCB, which offers low-volume board fabrication and single-sided assembly services. Below are notes for how we generated fabrication data.

Gerbers

Gerbers can be generated with the typical KiCad flow.

Part numbers

In the schematic, we added a LCSC field to all components, containing the JLCPCB part numbers. To generate the pick-and-place parts: in the schematic editor, go to Tools menu > Generate Bill of Materials..., run bom2grouped_csv, which produces a slider.csv in the project directory. This should have an LCSC column with the JLC part numbers.

Rename columns as follows:

• Reference -> Designators
• LCSC -> LCSC Part #
• Value -> Comment
• Other columns can be left as-is

Note: this was built against an older JLCPCB sample BoM file which used the column name LCSC Part #, instead of the JLCPCB Part # used in a newer sample BoM.

Positions

In the layout editor, go to File menu > Fabrication Outputs > Footprint Position (.pos) File... Since JLC does one layer only, select "Separate files for front and back". This creates a slider-bottom-pos.csv (and top file that can be discarded) in the output directory.

Rename columns as follows:

• Ref -> Designator
• PosX -> Mid X
• PosY -> Mid Y
• Side -> Layer
• Other columns can be left as-is

Optionally, correct rotations on parts. While we've sent in fabrication data with obviously wrong rotations (eg, TSSOP-20 oriented 90 degree off) and didn't get obviously wrong PCBs back, you can correct the rotations using a spreadsheet tool like Excel:

• Rename Rot to something different, eg KiCadRot.
• Add a RotCorrection column or something, to be manually set for each part. Positive rotation is clockwise (unmirrored view, at least on the bottom layer).
• Add a Rotation column, set to the formula of the KiCadRot cell plus the RotCorrection cell. This is the column containing the actual fabrication data.

Ordering Notes

In the PCB options, choose:

• Upload gerbers
• PCB Qty: as desired
• Surface Finish: ENIG-RoHS
• Gold Fingers: Yes
• 45 finger chamfered: No (ideally yes, but the board is too small)
• The defaults for the rest are fine

In the SMT Assembly options, choose:

• Assembly bottom side (the side with the QR code)
• Tooling holes: Added by JLCPCB
• Click "confirm"
• Add BOM File -> upload the slider.csv file (schematic BoM)
• Add CPL file -> upload the slider-bottom-pos.csv file (layout footprint position)
• Click "next"
• Review the component table
• Click "next"
• Review the placed preview, and fix footprint data as necessary (red dot indicates pin 1?)
  • If you need to go back, there is a not-at-all-obvious grey "< Go back" link at the bottom left of the page
• Review unselected parts: these are parts that will not be placed and should only be top-layer or other items to be manually soldered, card edge connectors, and mounting holes
• Click "save to cart"

Stencils:

• From the shopping cart, "Add new item"
• At the top, select the SMT-Stencil tab
• Upload gerbers, same as the PCB
• Stencil Side: Top & Bottom(On Separate Stencil)
• Stencil Qty: 2 (default)
• Fiducials: Etched Through
• Click "save to cart"