Panelization for DirtyPCBs

@DrAzzy you mentioned here about making your own panels in PCBs. Just wondered if you could elaborate a bit?

For the cut out in Eagle, do you just extend the board outline around? Do you make the board outline itself a specific width? And what do you put in for the rat bites? Just holes? Of any particular size?

Also, how do you put multiple brd files together? Do you do it with CUT/PASTE commands every time you change something, or some other way?

I've just been wanting to do a board full of Pico adaptors, but haven't put more than one board in one design yet.

Following from the other discussion. The 5x2 header looks a lot like Olimex UEXT.

The way I've been getting panelized boards from my dirty hookup in china is thus:

• Board outline encompases the whole 5x5 or 10x10 cm area.
  
• I start by making all the designs in one sch/brd file. If putting multiple copies of a design on one panel, yeah, I do copy/paste, which is annoying. I'm pretty sure there is a better way to do this, I just don't know it. When I had to make a panel with multiples of my tiny 85 project boards ( https://www.tindie.com/products/DrAzzy/attiny85-project-board/ ), since you can't just copy/paste everything in board ("please do this in schematic"), I copy/pasted just the traces, and then copy/pasted the parts in schematic, and positioned them appropriately using the traces as a guide - Naturally, eagle got really confused and said everything was unconnected and overlapping, but the boards came out fine.
  
• I draw the lines between them on the milling layer. I haven't pushed it to see how thin they'll let me make the cuts between the boards, I think I've used .032, .04, .05" widths.
  
• I leave gaps in the milling layer for the ratbites, and make them with a couple of small holes in a row.
  
  

I sent you a .sch and .brd via PM that show an example of a panelized board (the CH340G boards - not some of my best work, for a variety of reasons)

@cwilt - I think you meant to post that in the other thread?

I've done something similar with Dfrobot, their prices are similar and they've been decent quality, would recommend.

Thanks for the guide @DrAzzy, sounds like you've got it down to an art.

Thanks for all the info - I'll give it a go and see what happens!

If anyone is interested, I looked in the brd file and your ratbites are 0.5mm drill holes.

I'm not sure if this is useful, but when doing the Pico the second time, Jaltek wanted me to panellize everything for them. I never actually ended up doing it, but I was fiddling with Eagle script files for it.

They look a bit like this, and you use them with a command line like eagle -Spanel.scr panel.brd

# Kill all current contents
DISPLAY ALL;
GROUP ALL;
DELETE (c > 0 0);
# Set up board
GRID mm;
DRC LOAD ./espruino.dru;
CHANGE DRILL 0.3302;
SET WIRE_BEND 0;
# Add boards
DISPLAY NONE Top Bottom Pads Vias Unrouted Dimension tNames bNames;
PASTE R90 a_board1.brd (13 20);
PASTE R90 a_board2.brd (34 20);
PASTE R90 a_board3.brd (55 20);
PASTE R90 a_board4.brd (76 20);
# add wire
LAYER Bottom;
WIRE 'VCC' 0.2032 (3 11.25) (87 11.25);

It never actually goes near the schematic file, but you end up with a stand-alone board file containing all the sub-boards.

If I do something with the Pico adaptor shims I'll have a go at doing it that way - it'd be nice to have a clear, reproducable way of getting stuff in a panel.