Free? Panelising is never free. It always costs either money or time. Sometimes both if you screw it up.
1 Like
I would imagine for a proper production run you’d partner with your CM. They’d absolutely know best about how to optimize your panel for their equipment.
But for limited small batch runs like this (I only need 3 panels of my design) it makes more sense to just handle it myself based on whatever info the CM provides.
OSHPark, for example, uses 100mil (2.54mm) routing, 100mil (2.54mm) tabs, and recommends 2mil (0.05mm) mousebites spaced 4mil (0.1mm) apart center to center. (good grief I wish everyone would just standardize on metric).
1 Like
Hi,
Newbie to this forum, my 2 cents about using KiCad to do panelising gerber works.
I actually panelized my own board recently using KiCad. Here is how I did it.
-Before you design board, find out actual big PCB your board shop can do, find out that X * Y ratio if possible. Design your board according to that ratio (example is 18 x 24 inches), if your individual PCB near that ratio, it can fit better thus giving you cheaper $$. ( like 3.6 x 2.4 inches , or 1.8 x 1.2 or 1.8 x 4.8 … or etc etc), you get the idea…
-I finished routing the single board. DRC them make sure nets are properly connected. Define where the (0,0) of the PCB needs to be.
-Closed the job, save did all necessary PCB works.
-Working out the array pitch of each unit. Find out the spacing you intent to keep individual PCB apart, if you need to route (cutting by spinning bit) the board, diameter size of router is needed, so you have the size of PCB + router bit diameter = pitch. If you use v-score , the spacing can be zero or + 10mils (0.25mm) , pitch is basically XY length of the PCB. Always keep them as close as possible (save$$) , unless you have connector next to each PCB (overhang).
-Go into grid setup of the KiCad, inside the user defined grid, enter that XY grid. Switch over to this grid. Close the program.
- Open up just the pcbnew program. Do append PCB. Browse to the PCB job you just did. Start placing the first PCB at the (0,0) according to your original design , repeat the process for the array of PCB, maybe 3 x 4, 2 x 4, or 4x4 etc.
- After you have appended everything. Just output the gerber like normal, you will see the gerber produced is in array panel format. Even drill bit output are in array.
- Bare in mind , you will see a lot of ratnets disconnected (Due to the same nets disconnected- ignore it),
- This job does not include adding extra breakaway tab . You can add in writing for requesting Fab shop to add tooling hole + fiducial outside the PCB.
-If you needed more fancy panel outline design, perhaps do DXF export, then use LibreCad (2D) Cad editor to create the exact outline. Add in dimensional information.
I have done my board in that manner, economical and easy within your control. If you change your design, you need to repeat the process from start.
Ching L. Ooi
1 Like
I forgot to mention that, for routed PCB, you need mouse bit information added too. Board shop can help you on that dimension, it needs some drilling /v groove across the tiny PCB area that hole them in place after router cutting process…
1 Like
Highlight in the FAB drawing that the boards are to be penalized and shipped in array. Also mention the precise array size. Number of boards in array and spacing between them, tooling/fiducial requirement and railing details. If not the manufacturers will create a standard array drawing/Gerber based on your board dimension and thickness. Later they will send it for your approval before manufacturing.