Skip to content

Latest commit

 

History

History
101 lines (66 loc) · 5.27 KB

README.md

File metadata and controls

101 lines (66 loc) · 5.27 KB
Raw

Marble board scripting and processes

When a new design version of Marble is ready for manufacture, a release is tagged in this repository and the corresponding artifacts are made available for download (e.g. manufacturing package, documentation, etc.). We want the physical boards to have a QR code on them, pointing to the board's tagged release on GitHub. This way a physical board can be mapped to the source code and fabrication package that was used for its manufacture.

Updating the QR code for a new release, updating the silkscreen design accordingly and generating a fabrication package is a process in itself. That and other processes are partially scripted and documented here.

Generating the manufacturing package

If you have made changes to the Marble design and are ready to generate the manufacturing package, the first step is to pick a version number for the new release. The current version is v1.4.1.

Required software

KiCad version 6 is needed. We hope this still supports reproducible fabrication package builds. This means byte-for-byte identical zip files, independent of which person and computer runs the process.

Update the QR code on the silkscreen

The QR code needs to be re-generated so it points to the new version release. To update the URL, edit the Python script used to generate the QR code image: design/scripts/qr_create.py. The URL in that file pointing to the current release is: https://github.com/BerkeleyLab/Marble/releases/tag/v1.4.1.

From the design directory, run the Python script:

$ python scripts/qr_create.py

That will create a mm_qr.png file, which you should be able to preview and scan with your phone to confirm it has the intended link.

Open the KiCad project: design/Marble.pro

Open the Bitmap to Component Converter clicking on this button at the top of the screen:

Bitmap to Component Converter

Click on Load Bitmap and select the mm_qr.png that you just generated with the Python script. Choose 400 x 400 DPI to get a 19.8 mm output size. Check the Negative and Front silk screen, click Export and select logos/QR.kicad_mod to replace the previous QR code with the new one. You can now close the Bitmap to Component Converter and insert the QR code into the silkscreen.

Open the PCB Layout Editor clicking on this button at the top of the screen:

Pcbnew

Press the b key to fill copper planes (completing connectivity and getting rid of rats-nest visual clutter), and unselect every layer on the right-hand side except for F.silkS. There's a nice "Hide All Layers" feature available by right-clicking on the layer list.

Select the QR code, right click and select Update footprint.... Click Update and Close.

The above instructions are tested with KiCad 6.0.11. Be aware of KiCad issue #6514. If the results look corrupted and you are not able to scan the QR code from the PCB layout editor, select Modern Toolset (Fallback) under KiCad Preferences.

Generate the manufacturing package

Now that you have the updated QR code on the silkscreen, we're ready to generate the manufacturing package. The process is summarized in the diagram below.

The current design does unfortunately have a baseline of four DRC errors: overlapping courtyards of part pairs (U57, U62), (U32, U64), (U17, U63) and copper edge clearance for J10. These are INA219 chips with two package options supported with two (overlapping) footprints.

From the design directory, run:

$ bash scripts/manufacturing.sh

If everything worked out correctly, the script should have generated the fabrication package in a zipped archive containing the usual manufacturing files for both PCB fabrication and turn-key assembly:

  • Gerber
  • Drill
  • IPC-D-356
  • Board stackup
  • BoM
  • X-Y placement
  • Schematics

The above process is summarized in the diagram below.

process

Xilinx constraint file

A somewhat specialized tool is available to create an XDC file for the Marble design, based on a netlist file exported from KiCad.

From KiCad (version 6.0.x), open the Schematic Layout Editor clicking on this button at the top of the screen:

Pcbnew

  • From the top menu, select File / Export / Netlist
  • Select the OrcadPCB2 tab, click on Export Netlist and Save. The result shows up as Marble.net
  • If the above netlist was saved in the design directory, from the command line run:
$ python3 scripts/netlist_to_xdc.py Marble.net

The result shows up as Marble.xdc, which can be used for your FPGA designs.

Update I2C subsystem diagram in schematics

Run the following command from the top level directory before importing the I2C subsystem diagram into the I2C_MUX.sch schematic:

$ convert docs/marble2_i2c.eps -scale 1840 marble2_i2c.png

where convert is part of ImageMagick (Debian and derivatives: apt-get install imagemagick).