Hi Julia,
I can tell you how I’m dealing with Panelizing stuff:
for the first run, I order panelizing by the PCB manufacturer, and at the time I do specify panel configuration which is worked out with my EMS (single board configuration like 4x4, separation technology (v-score,route), margin size, additional fiducials and tooling holes for the margins),
I request the PCB manufacturer to send me back GERBER files for the combined panel (that’s the key here),
I prepare stencils for this particular panel design,
if for some reason I need other PCB fab to manufacture my boards, I do provide them the working GERBER files of the configured panel instead of just basic board design.
It would be harder to end up with identical panels, if the panel would be redesigned. You don’t have to change the stencil each time you choose new PCB manufacturer, and you can keep all your manufacturing configuration (like pick&place, AOI etc…).
Btw, I might have mistaken you with someone else, but does your entry mean that Gen16 brain is designed with Kicad?
That’s my process too. If they won’t send back Gerbers, its likely not the place you want to go. After all, you need to do a sanity check if they modify your files to make sure they didn’t mess something up.
Thanks for the great info. Yes, I’m the designer of the Gen-16 system; I used Express PCB for that project, it’s my favorite PCB tool by far for its great intuitive UI but it’s limited in some ways - you have to pay extra for Gerbers, you cannot get centroid data, routing signals on inner layers is difficult, you’re limited to 4 layers, 90-degree rotations, only circular holes, and no npth holes. I think our CM in China copied my layouts into PADS for final production.
Nice to hear you’re the designer of this breakthrough system.
IMHO Kicad seems a way to go. Few years ago I was looking around to find best low-cost EDA package that will allow me to do commercial projects. I chose Kicad and I’m pretty happy with my choice, especially after the project underwent massive improvement thanks to the dev team.
Kicad will not limit you with your projects, and with the features like interactive routing you’re getting close to the top tier EDA experience. Once you’ll learn it’s interface, it becomes a very handy tool. I’m successfully manufacturing Kicad-designed boards, and I don’t feel the need to look for alternative.
One more hint, use some 3rd party GERBER viewer for validation of your production files, just in case you’d find some “hidden feature” of the GERBER engine in your EDA package I use GERBV (part of GEDA package), and I’m fine with it.
Yeah, Kicad is OK, and generally less user-hostile than most other PCB programs like the absolutely ghastly Eagle. It’s just a shame that it contradicts so many standard (outside of engineering, anyway) UI paradigms; it’s really not necessary, as Express PCB demonstrates. The UI inconsistency between modules is a bit maddening as well, but I guess that’s to be expected from something written by various random people.
I’m enjoying the interactive router and tolerating everything else, although I still swear at it regularly.
Looks like it will do everything I could ever want, and well, with a pretty nice UI. Note that it’s not a stand-alone, you have to also buy one of their “main” CAM tools. I bought ViewMate Deluxe for $95, total investment was $350 for the package - a lot less than FAB 3000.
I’m glad you found a reasonable commercial solution. I may look into that myself.
If anybody finds this thread looking for a open source/hobby solution I have used gerbmerge multiple times before on kicad and eagle exported gerbers. One of the same or many unique designs are possible. I didn’t write the program, but my fork has some fixed for metric units that are needed to process kicad gerbers. The gerber processor is pretty basic, so it can have trouble with complex fills and slots. Opening and resaving in gerbv to simplify the gerber syntax can help. https://github.com/ihartwig/gerbmerge
I create my panels using the Append Board feature in Pcbnew. I am using tabs to connect boards together. This means I use a footprint that represents a tab and place it around the board that I have imported, modify the cut lines. Then I use the Create array feature to multiply the boards. As a last step I create the frame for the panel.
The final panel ends up looking something like this:
I wish there was a better system inside KiCad where one could just list some parameters of how the panel should look like. Making it easier to update the boards inside the panel, as well as creating new panels.
Yeah I obviously do not need that feature badly enough to implement it yet. But if the block reuse feature gets implemented that the developers are talking about on the mailinglist, the step to panelization will become much smaller.
Hey esden, thank you so much for posting that image. Your post told me everything I needed to know in order to start panelizing in kicad.
The trick was to create a new footprints for the horizontal and vertical 0.1" tabs with the mousebites.
For the mousebite/tab footprint, I started with a 0.1"x0.1" silkscreen box centered on the origin, so I knew where the margins are for the tab. Then I used 2mil (0.05mm) drills inset from the edge of the “tabs”. After those are set up, I erased the silkscreen and saved the footprint. I’m not sure if I have the drill size and mousebite offset perfect yet, but it’s a start.
(updated with correct mousebite drill specs, 2mil (0.05mm))
I leave panelising to the CM doing the board assembly - I just send them my cad files and I get back fully assembled pcbs.
In fact, I recently asked them if it would be better for me or them to panelise:-
Reply from the CM: “Yes best if you leave the panel design to us so we can optimise design for our systems and also to ensure its cost effective for a fabricator.”
Your CM probably wants tooling holes and panel sizes to suit their machinery - letting them panelise solves all this.
It’s certainly a good idea to talk to your CM about their process requirements, but not all CMs can or want to panelize your boards, especially for free.
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).
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
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…
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.
I use GERBV (part of GEDA package), and I’m fine with it.
