Panelising a PCB

Post Reply
parkview
Guru Maker
Posts: 603
Joined: Tue Jun 24, 2014 8:25 pm
Location: Busselton
Contact:

Panelising a PCB

Post by parkview » Tue May 11, 2021 3:38 pm

For most of my simple PCB's, I use this wonderful stand alone software utility to create 10cm x 10cm panels of smaller PCB's: http://blog.thisisnotrocketscience.nl/p ... panelizer/. In one of my recent PCB's: viewtopic.php?f=9&t=2457, I managed to fit 48 small PCB's into a less than 10cm x 10cm panel. So at current prices, five PCB's cost around A$19, which will give me a total of 240 PCB's at a cost of around 8 cents each. Nice!

So the workflow in KiCAD is to design up the PCB and export the 2 or 4 copper layers, plus front/back silkscreen and the front/back mask and the edge layers. I make my own stencils at home laser cutting 0.1mm acetate sheeting that I purchase from Jacksons, a local art store (A$9 for a A1 sheet).

From the exported layers, I change the *.gm1 file extension to *.gko, as sometimes the Gerber Panelizer software won't export the layers correctly.
Gerber-Panelizer.jpg
Gerber-Panelizer.jpg (49.41 KiB) Viewed 4334 times
I open the Panellising software, click File | New, to initialise the software. Sometimes I need to go to 'Panel Properties' and change the distance between boards to 2.1mm. It's not currently recommended by JLCPCB to go under 2mm if your using routed PCB's that I like to use for their nice rounded corners.
Panel-properties.jpg
Panel-properties.jpg (19.63 KiB) Viewed 4334 times
To add the initial PCB Gerber, you click on 'Board Placement | Add Gerber Folder', once that's done (mine lived in a folder called manufacture), I right click on 'instance' and click 'Add Instance'. I do this for as many as can fit into a 10cm x 10cm PCB. In this case, 239 times - whew!
add-instance.jpg
add-instance.jpg (26.16 KiB) Viewed 4334 times
Once that's all done, to automatically place all the PCB's, I click 'Board Placement | Autopack: Naive, where as the other option: MaxRects might fit some in sideways. You can move things around manually using the RH side interface, but it can be cumbersome.

Once I am happy with the board placements, I click: 'Breaktabs | Create Breaktabs' to automatically install mousebites between all the PCB's. Personally, I delete all the central ones placed at the junction of each PCB. You can also manually place breaktabs too if you need/want. I sometimes move them around to better fit board layouts. I don't want a breakout to be fitted over a USB connector, as I would then have to breakup the PCB before assembling it.

Once I am happy with it all, I can export the merged panel via: 'File | Export merged Gerbers' It's very funky, as I also generates a front and back view of how the panel is going to look. Look it over closely to make sure your happy with it all. Then zip us the nine new gerber files and upload to the PCB manufacture of your choice.

You can also save the Panel layout: 'File | Save'. If you don't change the PCB edge layout, then if you want you can re-export a modified copper/mask layout and just re-export the panel again, saving time.

In my opinion, the could be improved a bit by remembering the last folder that was opened, instead of me having to drill down the project folder tree every time, but hey, this sure beats manually creating mousebites like I have had to a few times for strange shaped PCB's.

parkview
Guru Maker
Posts: 603
Joined: Tue Jun 24, 2014 8:25 pm
Location: Busselton
Contact:

Re: Panelising a PCB

Post by parkview » Tue May 11, 2021 4:01 pm

So I received a panel of PCB's back the other day with it being the first time I have needed to cut up a stencil for the entire panel. In the past, I usually break up the panel and individually stencil and make up each PCB. But having some 50 indervidual simple PCB's it was easier to make up a panel at a time.

So, to make-up a panel stencil, I opened up the KiCAD project and re-exported the usual layers, but this time I also ticked the Front Paste layer. Luckily I had saved the Panelzer project layout, so I could open up the project and re-run the panel export, which now included the combined stencil layer: *. gtp.

I opened this panel layer in KiCAD GerberView, and it all seemed to look ok:
Gerber-view.jpg
Gerber-view.jpg (72.27 KiB) Viewed 4333 times

So I had a go at exporting it all as a SVG file, however, when I imported it into my laser cutting software: Lightburn, it wasn't what I expected:
Export-SVG.jpg
Export-SVG.jpg (44.2 KiB) Viewed 4333 times

The USB connector pads had turned from rectangles into circles.

The other option was to print it out as a PDF and luckilly that imported really well into Lightburn and the Panel stencil was all to size.
Print-PDF.jpg
Print-PDF.jpg (53.29 KiB) Viewed 4333 times

In this case, I was soldering up 5 panels of 10 small PCBs. Each one has a SMD USB-Micro and two PH connectors on it. I did have to hand solder one-pinheader and a USB-A through-hole connector onto each, but that didn't take too long:
USB-connector.jpg
USB-connector.jpg (64.7 KiB) Viewed 4333 times

Post Reply