[Feature request] Add support for KiCad PCM

[alvarezb]

It would be wonderful if the SparkFun part libraries could be included in the KiCad PCM! Either via a json url that we can add, or integrated into the default packages (similar to the SparkFun panelizer plugin)

[nseidle]

I take it as a great compliment that you think we should be available via the PCM! Thank you. We would love to do this but are limited on time. If you have the ability to help us, we would be thrilled.

[PaulZC]

Hi Brian (@alvarezb ),

I took a quick look at how much work would be involved to add these libraries to the PCM. The key document is this one. As a minimum, we would need to:

• Restructure the libraries: move Footprints into footprints; move Symbols into symbols; move Footprints/SparkFun-3D-models into 3dmodels/Battery.3dshapes, 3dmodels/Camera.3dshapes, etc,
• Update all the footprints with the new path to the 3D models
• Investigate how much the SPARKFUN_KICAD_LIBRARY environment variable complicates things
• Add an icon.png
• Add metadata.json

For the zipping of the archive, we could re-use (e.g.) the Panelizer workflows.

It would be good to automate the SHA256 generation for the metadata, and maybe even the push to GitLab. For the Panelizer, I currently edit the metadata manually using the Package Metadata \ tools (packager.py) and then manually submit the Pull Request on GitLab.

From then on, each time we open an existing design, we'd need to update the paths to match.

In summary: adding this to the PCM is entirely possible, but it's quite a bit of work and would involve several breaking changes.

It's much much easier if you clone this repo onto your local machine and keep it up to date using (e.g.) GitHub Desktop. If you "Watch All Activity" on this repo, you'll be notified each time we push or merge an update. Then you can Pull and keep your local repo up to date. (That's what we all do...!)

Best wishes,
Paul

[PaulZC]

Thinking through the SPARKFUN_KICAD_LIBRARY environmental variable. What path should we actually use? What is the correct KiCad-compliant path for the footprint 3D model? How does it relate to the KICAD9_3RD_PARTY environmental variable? (Can we use a relative path and avoid the KICAD9 binding?)

There are only 14 libraries registered in the KiCad 9 PCM. What can we learn from those?

The Alternate Kicad Library was last updated a year ago. There are some very useful docs here which discuss the PCM_ library nickname prefix. There's also this issue.

I can't see when the KiKit library was last updated, but there is some useful info here.

Searching GitHub for KICAD9_3RD_PARTY, I found a link to the Espressif kicad libraries. But it looks like they stopped at KiCad 8. Also, it's not available through the PCM. Maybe it was at one time? They use paths like:

(model "${KICAD8_3RD_PARTY}/3dmodels/com_github_espressif_kicad-libraries/espressif.3dshapes/ESP32-C3-WROOM-02U.STEP"

Do those work OK in KiCad 9? To find out, I installed the v3.0.2 zip file manually. I can see the symbols. The library has the PCM_ prefix:

If I add an ESP32-C3-MINI, I can see its 3D model OK:

even though it has the KICAD8 path:

OK. Good. KiCad must handle the KICAD8 to KICAD9 translation automatically. So it looks like we should be using 3D model paths like:

(model "${KICAD9_3RD_PARTY}/3dmodels/com_github_sparkfun_sparkFun-kicad-libraries/LIBRARYNAME.3dshapes/NAME.STEP"

[PaulZC]

But now we need to think through how this effects us (SparkFun) if we're using Git to stay up to date and don't have the libraries installed in the official KiCad\9.0\3rdparty folder

[PaulZC]

OK. Here's a plan that should work:

• Move the Symbols into symbols
  • Remember that Git is funny about case-only changes. You'll need to: delete Symbols, push, restore as symbols, push.
• Likewise, move Footprints into footprints
• Create a new folder 3dmodels. Create a new sub-folders Battery.3dshapes, Camera.3dshapes, etc.
• Move all of the SparkFun-3D-models into those new sub-folders
• Use VSC to change all of the footprint model paths:
  • Replace:
  • (model "${SPARKFUN_KICAD_LIBRARY}/Footprints/SparkFun-3D-models/
  • with:
  • (model "${SPARKFUN_KICAD_LIBRARY}/3dmodels/Battery.3dshapes/
  • (model "${SPARKFUN_KICAD_LIBRARY}/3dmodels/Camera.3dshapes/
  • etc.
• We have some rogue (model "${SPARKFUN_3DMODEL_DIR} which need fixing
• We have a rogue (model "${SPARKFUN_3DMODEL_DIR}/LED/Download_STP_WL-SFCC_150044M175200_rev1.stp which needs fixing
• In Symbol Editor, update your Preferences \ Manage Symbol Libraries. The Library Paths for all of the SparkFun libraries need to be updated. Change Symbols to symbols.
  • You can do this by deleting the libraries and re-adding them
  • Or you can cheat and edit C:\Users\<YOUR_USER>\AppData\Roaming\kicad\9.0\sym-lib-table. Replace ${SPARKFUN_KICAD_LIBRARY}/Symbols with ${SPARKFUN_KICAD_LIBRARY}/symbols
• In Footprint Editor, update your Preferences \ Manage Footprint Libraries. The Library Paths for all of the SparkFun libraries need to be updated. Change Footprints to footprints.
  • You can do this by deleting the libraries and re-adding them
  • Or you can cheat and edit C:\Users\<YOUR_USER>\AppData\Roaming\kicad\9.0\fp-lib-table. Replace ${SPARKFUN_KICAD_LIBRARY}/Footprints with ${SPARKFUN_KICAD_LIBRARY}/footprints

Once that is done, test a couple of designs in KiCad. Check that everything still works. You shouldn't need to update all the symbols and footprints. I think it should all be OK.

Now then. Here's where the fun starts. The above is OK for us (SparkFun). But what happens when we release the library through the PCM?

When I write the "Release Library for KiCad PCM" workflow, I will write it so that it goes through all the footprint libraries and updates the 3D model paths. The paths will be changed in the files in the release zip only. (The changes won't be pushed to the repo itself. That would be a disaster.)

• (model "${SPARKFUN_KICAD_LIBRARY}/3dmodels/LIBRARYNAME.3dshapes/
• will become:
• (model "${KICAD9_3RD_PARTY}/3dmodels/com_github_sparkfun_sparkfun-kicad-libraries/LIBRARYNAME.3dshapes/

With the icon and metadata, the library releases will then (hopefully) be ready to be included in the KiCad PCM. (We won't know for sure until we submit our first Pull Request...)

Once the libraries are in the PCM, users can install them with ease.

If a user downloads one of our board designs, the symbols in the schematic will have names like:

(symbol "SparkFun-Connector:Conn_01x05_P2.54mm"

If the user has left the Library nickname prefix set to PCM_, those symbols won't be recognised. The schematic editor will be expecting:

(symbol "PCM_SparkFun-Connector:Conn_01x05_P2.54mm"

So, unless I've missed something, I think we need to ask users to change (delete) the Library nickname prefix before they install the library.

Users don't have to do that. They could create their own schematics from scratch and the PCM_ prefix will be included by default. But they won't be able to edit our existing schematics, unless they add the PCM_ prefix to every symbol.

[PaulZC]

@nseidle : before we start any of the above, let's release the library as it is now, so users can revert if needed!

[nseidle]

@PaulZC - Release posted. Please have at it.

You'll need to: delete Symbols, push, restore as symbols, push.

Alternatively, you can rename to symbols1, push, rename to symbols, push.

rogue (model "${SPARKFUN_3DMODEL_DIR}

If these are from a recent commit, please let me know so I can mitigate it in the future (or talk to the engineer who needs to update folders).

[PaulZC]

Humm... Are we alone in facing the PCM_ nickname prefix issue? Nope. I'm seeing this exact issue discussed here by other library writers / maintainers.

We also need to deal with the "Footprint". Our symbols include Footprint properties like:

(property "Footprint" "SparkFun-Connector:1x05_P2.54mm"

But if the user has installed the library using the PCM_ prefix, the footprint properties need to be named:

(property "Footprint" "PCM_SparkFun-Connector:1x05_P2.54mm"

So, the workflow will need to search and replace all those too...

I think the following could work:

• Have the "Release Library for KiCad PCM" workflow create two zip file artifacts: one with PCM_ prefixes, and one without
• The metadata for the PCM will include a link to the with-PCM_ artifact
• Users installing the library through the PCM get a self consistent with-PCM_ set of symbols, footprints and models
• Add notes in the metadata description_full and each repo release, and include a link to the without-PCM_ artifact
• Users who want to open and modify our existing schematics (which won't have the PCM_ prefix) download the without-PCM_ artifact zip file and install it manually using the "Install from File..." option

We (SparkFun) keep using the library almost as is - except for the above Symbols/symbols, Footprints/footprints and 3dmodels changes - and keep using Git to stay up to date. Anyone at SF who doesn't want to use Git can install the latest without-PCM_ zip file release and use that.

[PaulZC]

Arggg...!!!

The 3dmodels folder should be structured as follows:

Battery.3dshapes
Camera.3dshapes
Capacitor.3dshapes
etc...

Do over...

[PaulZC]

Hopefully corrected in #235

[PaulZC]

Next problem...:

The capitalized .STEP extension is causing problems. Lower case .step is OK... Picky, picky, picky....!

Fixing...!!

[PaulZC]

Yabba dabba doo! We're in business!!

Pipeline is passing and the Merge Request is in: https://gitlab.com/kicad/addons/metadata/-/merge_requests/504

Release notes: https://github.com/sparkfun/SparkFun-KiCad-Libraries/releases/tag/v9.0.0