The stuff of Kryton

An eclectic selection of technology with some cookery

Project maintained by kryton-me Hosted on GitHub Pages — Theme by mattgraham

KiCAD-JobSet

Introduction

Some basic settings to get set up with Job Set, Please note this uses Unix / Linux / Mac file paths Windows users need to adjust accordinly

Variables

Set up the follwoing variables:

Project Defaults

Name Description
PROJECTNAME This is the file name of the project so may not that usefull.
CURRENT_DATE todays date

Variables to defined

THis is just my suggestion feel free to set it up your own way.

Name Description Notes
VERSION Issue of files being issued  
PROJECT# i.e. PCB-001  
PROJECT-DESCRIPTION Discription of the project  
COMPANY Company / Organisation responsible Embed in template if possible
BY Creator: MF or Mic F or M Faraday  
APPROVER Approver: see above  
VERSION-CURRENT Description of changes in that version  
VERSION-LAST Description of changes in that version  
VERSION-LAST+1 Description of changes in that version  
VERSION-LAST+2 Description of changes in that version  
VERSION-LAST+3 Description of changes in that version  
VERSION-LAST+4 Description of changes in that version  
VERSION-LAST+5 Description of changes in that version  
VERSION-LAST+6 Description of changes in that version  

Usage

A syntax example: ${PROJECTNAME} or ${CURRENT_DATE}

I’ve added Number which is not in the default template to comply with BS8888

Page Settings

THis can be skipped if the correct page templates are set up.

Applicable and SCH and PCB and Automated the title block of any drawing. | Variable on Sheets / Drawing | Applicable too | Applicable Variable | Notes | | — | — | — | — | | Issue Date: | Both | ${CURRENT_DATE} | | | Revision: | Both | ${VERSION} | | | Title: | Circuit | ${PROJECT-DESCRIPTION} Circuit Diagram | Extra “A” for assembly | | Title: | PCB | ${PROJECT-DESCRIPTION} Printed Circuit Board | | | Number: | Circuit | PCBA-${PROJECT#}-${VERSION} | Extra “A” for assembly | | Number: | PCB | PCB-${PROJECT#}-${VERSION} | | | Company: | Both | ${COMPANY} | | | Comment1: | Both | ${BY} | | | Comment2: | Both | ${VERSION-CURRENT} | | | Comment3: | Both | ${VERSION-LAST} | | | Comment4: | Both | ${VERSION-LAST+1} | This is the last displayed comment. | | Comment5: | Both | ${VERSION-LAST+2} | | | Comment6: | Both | ${VERSION-LAST+3} | | | Comment7: | Both | ${VERSION-LAST+4} | | | Comment8: | Both | ${VERSION-LAST+5} | | | Comment9: | Both | ${VERSION-LAST+6} | |

JobSet settings

Set up a file

Project tool -> File -> New Jobset File… -> Enter file name -> save

Destinations

Just one Desitination for Both PCB & PCBA

Name Value notes
Description: Output  
Destination path: ../Output Exact syntax with dots is impotant (Not tested on Windows)
Inclued jobs: tick them all Go back to check this once they are set up

GERBER with drawing

+ –> “PCB: Export Gerbers” –> “OK”

Name Value
Output directory: PCB-${PROJECT#}-${VERSION}/PCB-${PROJECT#}-${VERSION}-GERB
Inclued Layers: Top, Bottom, Silkscreens, Solder masks,, Past mask, Document Layer, & Multi Layer
General Options: Plot Drawing sheet, Check zone fills before plotting
Gerber Options: Use Protel filename extensions, Use extended X2 format

Actions:

GERBER no Drawing (JLC)

+ –> “PCB: Export Gerbers” –> “OK”

Name Value
Output directory: PCB-${PROJECT#}-${VERSION}/PCB-${PROJECT#}-${VERSION}-GERB
Inclued Layers: Top, Bottom, Silkscreens, Solder masks, Past mask & Multi Layer
General Options: Check zone fills before plotting
Gerber Options: Use Protel filename extensions, Use extended X2 format

Drill Data (JLC)

+ –> “PCB: Export drill data” –> “OK”

Note this uses the gerber folder so it’s with the GAERBER data in the same zip file. | Name | Value | | — | — | | Output directory: | PCB-${PROJECT#}-${VERSION}/PCB-${PROJECT#}-${VERSION}-GERB | | Fromat: | Excellon, PTH and NPTH in single file, use alternative drill mode for oval holes | | Options: | Orgin: Absolute, Units: Millimeters, Zeros: Decimal format (remomended) |

Actions:

IPC-2581

| Name | Value | | — | — | | Output directory: | PCB-${PROJECT#}-${VERSION}/PCB-${PROJECT#}-${VERSION}-IPC-2581.xml | | Inclued Layers: | Units:mm, Precision: 6, Version C | | BOM Columns: | Internal ID: Generate Unigue, Manufacturer P/N: Omit, Manufactrer: N/A, Distribution P/N: Omit, Disibutor: N/A |

ODB++

| Name | Value | | — | — | | Output directory: | PCB-${PROJECT#}-${VERSION}/PCB-${PROJECT#}-${VERSION}-ODB | | Inclued Layers: | Units:mm, Precision: 4, Compression: ZIP |

PCB Drawing / Specification

+ –> “PCB: Export PDF” –> “OK”

Name Value
Output directory: PCB-${PROJECT#}-${VERSION}/PCB-${PROJECT#}-${VERSION}-SPEC.pdf
Inclued Layers: Document Layer
Plot on All Layers: Top, Bottom, Silkscreens, User Comments & Multi-Layer
General Options: Plot Drawing sheet, Check zone fills before plotting
PDF Options: All

Actions:

PCB Pick and Place file

WARNING: Make sure all copper compnents & PCB shapes / specs are marked “Do Not Populate” Components with “180.000000” appear to have the wrong polarity. to many digits? + –> “PCB: Export Position Data” –> “OK”

Name Value
Output file: PCB-${PROJECT#}-${VERSION}/PCB-${PROJECT#}-${VERSION}-PAP.csv
Format: CSV
Units: Millimeters
Tick boxes: Exclued all footprints with the Do Not Populate flag set, Inclued Board edge layer, Generate single file with both front and back positions

Actions This may need editing to be compatible with a manufacter [such as JLC](2026-02-KiCADToJLC]

PCB: 3D Model

+ –> “PCB: Export 3D Model” –> “OK”

Name Value
Format: STEP
File: PCB-${PROJECT#}-${VERSION}/PCB-${PROJECT#}-${VERSION}-3D.step
Board Options: Export board body, export silk screen, Export components (All)
Coordinates Board center origin
Other Options Substitute similarly named models, Don’t Write P-curves to STEP file

Schemtic (SCH) PDF

+ –> “Schematic: Export PDF” –> “OK”

Name Value
Output directory: PCB-${PROJECT#}-${VERSION}/PCBA-${PROJECT#}-${VERSION}-SCH.pdf
Options Page Size Schematic size, Plot Drawing sheet, Output mode color, color theme KiCAD classic
PDF Options Generate property popups, Generate clickable links for hierachical elements

Actions

Bill of Materials (BOM)

+ –> “Schematic: Generate Bill of Materials” –> “OK”

Name Value
Output directory: PCB-${PROJECT#}-${VERSION}/PCBA-${PROJECT#}-${VERSION}-BOM.csv
Edit Select View Preset
Export Format preset: csv

Actions:

Process