= How to work with an electronics project =

 1. Plan the connection in a system diagram

   * What is the form factor of the input and output connectors
   * How the connectors are assigned to the front and rear panels
   * Assign reasonable panel labels

 1. Panel design
   * Copy the past design files, as they are nicely designed for the LIGO chassis
   * If the PCB is directly mounted on the panel, be aware that the connector height needs to be precisely adjusted.

   * Arrange the connectors and the labels as planned in 1.
   * Is the planned connector assignment physically feasible?
   * If not, how should the assignment/arrangement be?

   * Once the design is done, reflect the modification in 1.
   * Save the panel files. Export the design in PDF and STP

 1. SCH/PCB design in Altium
   * Copy the past files depending on the # of layers (usually 2 or 4 layers)
   * First of all, copy the files and open them in Altium, then rename the file names.

   * Approximately design the circuit.
   * Look at the PCB file and remove all the components from the PCB (except for the PCB outline)
   * Use "Design/Import Changes From ....PrjPcb" to force the consistency between the SCH and PCB. Always incorporate the change into the PCB.
   * You'll face a bunch of errors because there are missing footprints. Update the library.

   * By the way the paper size can be changed from the "properties" panel of the schematic by selecting the templates.
   
   * '''How to make a library for the missing parts'''
      * Go to the "Manufacturer Part Seach" panel. 
      * There, search for your favorite component. The component has to have a green IC chip mark (i.e., has a 2D/3D footprint model)
      * Click the component photo to download the model. It is downloaded to somewhere weird like c:\Users\Public\Documents\Altium\AD21\Library\ExportIntLib\
      * Extract the zipped library. Open xxxxxx.LibPkg. It contains PcbLib and SchLib.
      * Go to the downloaded SchLib and copy the component to your SchLib. The component has a strange name, so this is the chance to change the name for your convenience.
      * Go to the downloaded PcbLib and copy the component footprint to your PcbLib. The component has a strange name, so this is the chance to change the name for your convenience.
      * If you change the footprint name, the link between the component and the footprint is broken. Correct it by adding the footprint in the SchLib.
      * Try to incorporate all the 3D models into the parts as much as possible. It will help to match with the panels in the assembly confirmation below.

   * '''Board Outline in the PCB mode'''
      * Change the board size in "Board Panning Mode" with the shortcut key "1". BTW, "2" and "3" are the 2D and 3D modes.
      * For the standard 19inch LIGO units, the board width is expected to be 14000mil. Use the dimensions to align the connectors along with the panel design.

   * Some keywords
      * "Rooms" to duplicate the PCB pattern over the repeated channels
      * "Polygon" pouring to check how the polygons are filled
      * Always use "DRC Check" to find possible overlap, missing wiring, etc.
      * Look at the part information in the property to see what parts are linked to the SCH symbol. Often the parts are not in stock for the old PCBs.

 1. Assembly
   * Once the PCB is ready, export the 3d model with the STEP format. Note that the single part option has to be used.
   * Export the panel designs into STEP too (.stp).
   * Go to Solidoworks. Open these STEP files and they can be saved as SLDPRT files so that they can be included in a assembly file.
   * Use D2000573-v1_105kHz_ADC_Interface_1U_Chassis.SLDPRT as the chassis template.
   * Include the parts files and mate them as we want.
   * Check if the panels are well matched with the PCB connectors.

 1. PCB ordering
   * On the PCB design in Altuim, select Fabrication Output/Gerber Files
      * Use 0.01mil option
   * Then select Fabrication Output/NC Drill
      * Use 2:4 option
   * The files are in the Project Output Folder
   * Zip it and upload to JLCPCB.com
   * JLCPCB will check the design once the payment is done. Their minimum order Qty is 5 PCBs per design. They only accept credit cards.

 1. Documentation
   * Create a PDF file for the SCH, PCB, and BOM by SmartPDF
   * Create PDF files of the panel designs.
   * Use Reports/Bill of Materials to create a BOM excel file
   * Upload files to DCC
       * SCH/PCB/BOM PDF
       * Panel PDFs
       * BOX excel 
       * Zipped gerber files
       * Zipped project files
       * Front Panel Express: Panel design files (fpd files)