V-Score layer selection not working correctly

[tcurdt]

I am trying to send some PCBs to JLPCB.
Seems like Fabrication Toolkit wants the v-score on layer User.1

Unfortunately selecting the layer in this plugin does not put the v-scores into that layer.
And re-opening the dialog it selects multiple?!

[PaulZC]

Hi Torsten (@tcurdt ),

Thanks for reporting!

You're taking the Panelizer into unchartered territory... AFAIK, we've never tested the Panelizer with the Fabrication Toolkit so I don't know how well they will work together. We use our own CAMmer to generate the Gerbers for JLCPCB.

But it's clear you have revealed a bug - by having more than 9 User layers turned on. I don't think we ever use that many. There must be a flaw somewhere where selecting User.1 causes anything starting with User.1.. to also be selected. I will have to dig through the code to find that...

Best wishes,
Paul

[PaulZC]

@tcurdt : can you please post the contents of the panel_config.json and panelizer.log files. Thanks!

[tcurdt]

Hey Paul

You're taking the Panelizer into unchartered territory... AFAIK, we've never tested the Panelizer with the Fabrication Toolkit so I don't know how well they will work together. We use our own [CAMmer]
(https://github.com/sparkfun/SparkFun_KiCad_CAMmer) to generate the Gerbers for JLCPCB.

So many options. I've always use FT but now also found Gerber To Order - and now CAMer :)
TBH I don't care much which to use but guess it should not really matter that much for Panelizer.
Just a question how to communicate the v-score to JLCPCB.

And TBH I am not even sure what they expect yet and what this means for the panel settings on upload.
First time I try this.

But it's clear you have revealed a bug - by having more than 9 User layers turned on. I don't think we ever use that many. There must be a flaw somewhere where selecting User.1 causes anything starting with User.1.. to also be selected. I will have to dig through the code to find that...

Yes, that's also what I figured.

It seems it works for most layers - but not User.1

can you please post the contents of the panel_config.json and panelizer.log files. Thanks!

Sure thing. Attached.

panel_config.json
panelizer.log

[tcurdt]

Another thing I noticed. It actually creates many small PCBs instead of a single one with v-cuts. At least JLCPCB told me that's wrong.

[tcurdt]

IIUC they expect something more along the lines of this?

[PaulZC]

Hi Torsten,

Yes, that's all true. But we regularly have PCBs made by JLCPCB using the zipped Gerbers produced by the CAMmer. We're open about the Panelizer's limitations in the README. Maybe JLCPCB can work with our panels because both edge cuts and v-score are merged into a single GKO file? Or maybe they have a "Remove redundant SparkFun edge cuts" button they always hit when we send them a new design? ;-) I can understand them being confused if you send them the v-score lines separately. Also, our panels always have a border so we can clamp them down on the Pick and Place machine. Maybe that helps too?

Best,
Paul

Edit: just adding a link to the notes in the code:

SparkFun_KiCad_Panelizer/SparkFunKiCadPanelizer/panelizer/panelizer.py

Lines 692 to 701 in ed898dc

	# SFE: On SFE panels, we keep all the existing edge cuts and let JLCPCB figure out which are
	# true edges and which are v-scores. Also, if the edges are not straight lines, it gets
	# complicated quickly. (The original version of this panelizer only worked on rectangular
	# boards.) (Use KiKit if you want to avoid the redundant edge cuts.)
	#
	# Erase all existing edgeCuts objects (individual board outlines)
	#drawings = board.GetDrawings()
	#for drawing in drawings:
	# if drawing.IsOnLayer(edgeLayerNumber):
	# drawing.DeleteStructure()

[PaulZC]

Ah! I might have found it:

SparkFun_KiCad_Panelizer/SparkFunKiCadPanelizer/panelizer/panelizer.py

Line 368 in ed898dc

if V_SCORE_LAYER in board.GetStandardLayerName(i):

I should have used == instead of in...

[tcurdt]

Sorry for dragging you through my panelisation learnings here.

Yes, that's all true. But we regularly have PCBs made by JLCPCB using the zipped Gerbers produced by the CAMmer. We're open about the Panelizer's limitations in the README. Maybe JLCPCB can work with our panels because both edge cuts and v-score are merged into a single GKO file? Or maybe they have a "Remove redundant SparkFun edge cuts" button they always hit when we send them a new design? ;-)

IIUC a "GKO" layer is a silk screen layer? A recent JLCPCB support mail expected all v-score cuts to be in there.
Which supports your SparkFun button :)

But a previous person said the lines should be in the edge cut layer. Which is also what is in there docs:

The V-cut line should be the same as the outline of the Sub-PCB. That is to say, there is zero space between the sub-boards.

https://jlcpcb.com/help/article/pcb-panelization

...which KiCAD does not seem to like.

All 3 gerber exporters I tried (Fabrication Toolkit, CAMler, GerberToOrder) seem to do handle this slightly different 🫣
So sorry for derailing this ticket here a little.

Also, our panels always have a border so we can clamp them down on the Pick and Place machine. Maybe that helps too?

Support said that's only important for assembly. And if I don't order PCBA it's not necessary.
Just seems like the cuts need to be on the correct (whatever that is) layer.

I still have the feeling I am not getting the full picture but I was thinking about the edge cuts:
Why does the panelizer not remove them and just create a rect of the bounding box instead?
Wouldn't that also be an option? or at least another possible feature?

[PaulZC]

There's also a weakness here:

SparkFun_KiCad_Panelizer/SparkFunKiCadPanelizer/dialog/dialog.py

Line 164 in ed898dc

if value in self.vscore.LayersGrid.GetCellValue(row, 1):

I suspect this is what is causing the multiple ticks... I'll test this shortly.

[PaulZC]

@tcurdt : no problem. I'm happy to chat about this.

I added an "Edit" to my post above.

Panelization is 'easy' when you're working with close-butted rectangular PCBs. But if you need gaps between rows or columns of PCBs for overhanging components (like USB-C connectors), it gets more complicated. If the exposed edges have curved features, it gets much more complicated. I should say that KiKit handles all of this - very well. But it's a bit too complex for us. We prefer a simpler zip-and-go solution.

Also, this Panelizer is based heavily on the original Eagle Panelizer (dating back to 2018 or earlier). The way we use the Gerber files originates from that.

JLCPCB say they prefer the following Protel naming convention:

The KiCad Gerber Viewer thinks GKO is a soldermask / silk / outline layer. But that's not how we (SparkFun) use GKO.

The Panelizer also adds the text "ROUTE OUT" on any gaps that need to be routed / milled away. (Think wood router, not track auto-router...) This just makes it clear to JLCPCB which bits are PCB and which bits are gaps. Sometimes we forget and that causes much confusion.

Maybe JLCPCB are more forgiving because SparkFun have been buying lots of boards from them for years? Maybe they expect new customers to do things better? I'm not sure. All I can tell you is that we upload the zip file produced by the CAMmer, select "Single PCB", and we (almost) always get beautiful scored panels shipped out very quickly.

[PaulZC]

Hi Torsten (@tcurdt ),

I think I've resolved this. Please try the attached zip file. You will need to Uninstall v1.4.0, Apply Pending Changes, and install the v1.4.1 zip file manually (Install from File).

The CAMmer may have similar weaknesses. I'm taking a look now.

Best,
Paul

SparkFunKiCadPanelizer-1.4.1-pcm.zip

[PaulZC]

Hi Torsten (@tcurdt ),

Have you been able to test version 1.4.1? Does it work for you? Shall I release the changes?

Best,
Paul

[tcurdt]

Have you been able to test version 1.4.1? Does it work for you? Shall I release the changes?

Sorry for the late reply, Paul. Life got in the way.

Thanks for the test version.
I can confirm all the issues I had seem to be fixed. 🎉

Please feel free to close the issue once it's released.
Thanks for the quick help!