Skip to main content ↑ ↓
Topic: Panelizing PCBs (Read 6434 times) previous topic - next topic

Panelizing PCBs

I just wrote up an instructable (here: http://www.instructables.com/id/Paneliz ... ree-Light/) about how you can easily panelize PCBs for SeeedStudio's Fusion PCB service.  I thought it might be of some interest here, especially considering that they are currently offering 10 count 10cm x 10cm PCBs for the same price as 10 count 10cm x 5cm PCBs.

It requires a minor patch to gerbmerge, but after that, it works like a charm.

Re: Panelizing PCBs

Reply #1 –
Thanks, I have always wanted an overview of a gerber merging app
Got a question? Please ask in the forum for the fastest answers.

Re: Panelizing PCBs

Reply #2 –
very good information thanks

Re: Panelizing PCBs

Reply #3 –
It was a lot easier than I thought, the most nerve-wracking part was after submitting the initial gerbers (without the patch that drew the entire board outline) and getting a response from Seeed saying something to the effect of "are you sure this is what you wanted?  without a board outline you will get 2x the order, and we will charge your card for it.  give us corrected gerbers ASAP".

I'm glad you found it useful.  I won't mention how this instructable's entered in a contest, nor how you can go vote for it, if you find it worthy, very easily by looking at the banner near the top of the page.  That would be rather gauche, wouldn't it?

Re: Panelizing PCBs

Reply #4 –
I have updated the merging program to allow the user to add arbitrary text to the merged files.  I wanted to avoid having to put the Seeed order # on the silk of the board itself, before rendering the gerbers, so I could re-use the same gerbers if I wanted to order them again, and so that I didn't have to put the order number on each board, where it was visible.

Now it will try to put the text you specify in the space between the boards on the panel:
C:python.exe path/to/gerbmerge.py --text "SeeedStudio Order # 12345" panel.cfg panel.layout

It tries to automatically determine the text size based on the spacing between the boards, and it tries to automatically determine the stroke width based on the size.

You can also specify an exact X and Y for placement on the merged panel, an exact size, and an exact stroke, if the automatic ones don't give you the results you want.

It is not very smart about placement, it assumes you have at least two rows in your layout, and puts the text between the first two rows.  It probably wouldn't be too hard to make it pick the best place.  I'll probably add that feature when I need it.  It also doesn't handle rotation yet.

You can get the latest at:
https://github.com/space-age-robotics/gerbmerge-patched

It also adds a '--ack' flag, to auto-ack the 'no warranty' message that comes up (which makes scripting slightly easier).

Here's an example of the output:

[attachment=0]

Re: Panelizing PCBs

Reply #5 –
I sure that this is all nice and so, but why do you need a python script to panelize a a few copies of a board layout?

I simply run the built-in panelize.ulp to get my bottom/top silks on new layers so my part numbers won't auto-increment when I just copy & paste,paste,paste the design onto a new board a few times.

I set the grid on the new board to 0.5mm and paste the design with an extra space of 0.5 mm so I can put a tStop/bStop rectangle there for easier depanelizing with a large box cutter. The stop layers create a slight groove there that keeps the knife from straying off.

Actually, on my last batch of boards from Seeed they did a V-Score on my panelized boards where I had the tStop/bStop separator so I could just snap off the individual boards from the "panels".  That was a nice surprise....

I also had 9 boards on a 5x5cm pcb and they manufactured it without complaints even if they spec the max numbers of sub-boards on a single pcb is 5.

Re: Panelizing PCBs

Reply #6 –
For those on the free version of eagle, this script will allow a panel larger than the limitated size available (e.g., for a 10cm*10cm board at Seeed).

I have not been very successful using panelize.ulp. It was easy enough to get started with gerbmerge, and I have just been updating it to meet my needs.  I like being able to keep the gerbers for my design and make follow on orders with a different order ID, or with a different combination of boards on the panel.

Thank you for that idea about the stop layers, I'll have to look into that.

Re: Panelizing PCBs

Reply #7 –
[quote author="schazamp"]For those on the free version of eagle, this script will allow a panel larger than the limitated size available (e.g., for a 10cm*10cm board at Seeed).[/quote]
Ah!  That is a very good reason for not just copy/pasteing :-)

Re: Panelizing PCBs

Reply #8 –
I was using this more today, and thought I'd mention how it helped my workflow -- my PCBs were just slightly too large for the Seeed panel constraints, but gerbmerge told me that, and I was able to tweak the size, re-run the CAM job, and re-run the merge (thank you, command prompt history) to fix it, while maintaining minimum space between boards for sawing. 

I realize that panelizing by hand would have made the size problem readily apparent, but I prefer avoiding manipulating things with the mouse when it is avoidable.

Re: Panelizing PCBs

Reply #9 –
Speaking of depanelizing with a saw or boxcutter knife. It's so much easier to do it if you order boards with 0.8 mm thickness instead of the regular 1.6 mm.

same price at Seeedstudio, but lower shipping costs due to the lower weight. And unless it's a 10 x10 cm board with  heavy parts like a power transformer on it I don't see any issues with the board being too flimsy/flexible.

1.6 mm boards are so "two decades ago"  :-)

Re: Panelizing PCBs

Reply #10 –
Does any one tried software CAM350? You could use its panel tools, panelizing is a piece of cake.
I often do panelizing jobs for clients to save their time and money.
You could also panelize different designs into 1 panle to save costs.