I am making a small sensor PCB with SHT21 temperature humidity sensor that will be placed away from the main board. I want to isolate the sensor from the PCB board so I am trying to insert 2 slots around the sensor as on below image.
The thing is that the KiCad is not really allowing for this (or I don’t know how to do it). When I make a outline of the slots on the Edge.Cuts layer the 3D display crashes so i’m not sure that this would work in the PCB fab / gerber output. I’ve seen the tutorial on how to make oval slot holes but this seems clumsy and lack customization.
I’ve asked my manufacturer about this and got the reply: I think you can make an individual layer for it, and make a note in the design, say"plated slots or none plated slots"
So my final decision is to make a outline on the Eco1.User and make a note outside of the board area saying “NON PLATED SLOTS”.
Does anybody have the similar problem and have a better idea?
You probably got an error message about not finding a contiguous line or “next point” for the outline.
You can use the outline layer for slots (assuming the factory supports that), but you have to use EXTREME care that the line segments are contiguous, meaning the starting/end-points must be very close together, ideally be identical.
I suggest using the openGL mode for this, as is makes handling lines/arcs so much easier. This requires using a more recent version of kicad. The “old-stable” release doesn’t support it.
I’ve just downloaded new KiCad wininstall and will try this today in openGL. I can see that the slots on your board are straight. Did u try to make curved one like mine?
you can also do curved ones - but you have to do it manually:
you need to draw both sides of the slot - in your picture you draw just one line - that currently does not work.
I’ve tried it and it seems to be working. I’ve sent my board as per manufacturers recommendation though with cuts in a separate layer. Will see how this comes out.
I certainly did not know that the functionality depends on the mode of display. I have noticed that the tools are somewhat different when in openGL mode. Maybe this mode should be default.
I’ve downloaded and compiled today’s winbuild and will be testing it tomorrow.
The polygon points for cutouts need to be within about 0.25mm of each other to be accepted as a contiguous line. This is fairly easy to achieve in 45° and 90° geometries, but gets rather tricky if lines / arcs must match at odd angles. Frequent testing & using a very fine grid is helpful.
Drawing fancy coutouts in non-openGL mode is a futile task and will end in madness.
You can create curved cutouts by simply drawing the outline of the cutouts on the Edge.Cuts layer; the restrictions are (1) the outline must be a closed loop and (2) it must not create an isolated island within the board (split board into multiple solid bodies). I can’t remember if there’s an easy way to specify such a curved cutout but the structures certainly exist in pcbnew; I even generated curved plated-through slots as a test case while working on the VRML modeling 2 years ago. I’ve argued several times for a dedicated “cutout” layer but the other devs don’t agree that it would be useful.
I have a similar question - I’m creating a large ring PCB for a project which means the interior of the ring is devoid of copper-fill and without components. Such a waste when the fab charges you by the square inch. My intention is to make several nested rings to make better use of the area. However, when I create the edge cuts for the inner and outer diameter of the larger ring, it effectively makes the interior a wasteland with no copper fill.
I see in Madworm’s picture above something similar to what I’d like to do but he’s created a isthmus betwen the outer and inner board with what appear to be drills to aid in breaking away the inner board from the outer board.
I was led to believe that fabs don’t like to have exposed copper layers left from the routing process (creating the cutouts). Have you created an internal exclusion for the isthmus to ensure there is no copper exposed during the cutout process?
That’s why copper fills/pours are set back a bit from the edge.cuts - see their options when you create one.
If that’s not enough (or doesn’t give you expected results) you can also place no-fill zones… I think on the pcbs below some of those NPTH holes would have caused ripples/waves in the copper zone edge, so I placed no fill zones over some of them to get straight edges.
As for routing through a little bit of copper - I didn’t had problems the last two times I did castellations at Elecrow, where the router was going through PTHs for a short stretch (even 2 different fab houses, as certain details aren’t the same). Mind you the router was 1mm in diameter though… as those where at board edges - but you can see the copper pour stopped before the board edges at any case (top left, bottom right):
The footprints I used have the edge.cut layer marked on the cmts.user layer. I went for the biggest hole size I could get away with while still getting some copper around it on the pcb after considering accuracies of drilling etc. to stabilize the copper that is being cut away. As you can see on the picture, some PTH copper has not been cut but squeezed into the half-hole - it’s pretty easy to get that out with some sharp pointed tool. KiCADinfo_Castellations.pretty.zip (1.2 KB)
Afaik, the factory will treat completely separated pcb pieces - even if they come from one set of gerbers - as single pcbs and charge you more… thus people arrange them and keep them together, but make them easily separable. Some fabs don’t appreciate that and still charge you for separable pcbs though (more milling = longer time and more wear on router bits) but most Chinese fabs don’t care it seems (or it’s already priced in) and don’t charge you extra.
Another reason for this is if you want to use surface mount devices and have a solder mask made from the gerber set… it’s easier to handle the complete piece, rather than smaller ones, and break apart after reflowing the whole thing.
As for having the copper pour also on the inner parts that are separated by break-away-tabs - you need to have some footprints or tracks going there to connect the fill-areas with the nets. The tracks can traverse edge cuts, no problem, it just won’t look nice where they leave/enter the board.
Or you can put down a separate fill area for the inner parts as I did here - adjust the priority level in the areas options dialog when you do this, otherwise it won’t fill or even be create-able if it overlaps another one.
Do you have a screenshot of what you have in mind?
In any case, make sure that the lines/arcs on the edge.cuts layer meet each other down to 0.1 mm I think - check with gerber viewer tools to make sure your edge cuts are closed (some can’t deal with nested edge cuts though, look at the link where I posted some tests). For simple 90 deg shapes/corners this can be done in pcbnew, but for anything more complex you want a CAD program that exports dxf that you can import into pcbnew (above example).
You also don’t need to round any internal corner unless the radius shall be greater than half the diameter of the router bit being used (usually minimum of 0.8 mm possible, 1 mm and up are more common) - that’s why I have sharp corners in there (makes closing the edge cut loop a breeze and doesn’t affect the outcome).
@Joan_Sparky - Wow, what a great reply to a 7 month old thread I awakened to add my own problems to. I’m new to PCB design and new to KiCAD and this forum and the people like you and @madworm and others have been amazingly helpful - even by my just reading each of the threads I’ve already learned so much.
Castellations, Mouse-bites - just those two terms alone are going to help. Before I knew what they were called, it was difficult to search for information online about them.
And you mentioned being able to set a priority level for pours - I didn’t know you could do that or that it would help solve my problem. I had tried to create a nested zone inside of another zone but the nested zone wouldn’t draw so I assumed there wasn’t an option to do that and moved on to other solutions (like appending PCB designs into a single file - which I haven’t tried yet but found other forum posts discussing it).
As to the Fab charging extra - I already talked with OSHPark about this issue and they indicated it wouldn’t be a problem to nest boards and while the support person wasn’t specific, I got the impression they wouldn’t charge extra (they charge by the area even though I see your point about additional milling being an additional cost to the Fab).
So much cool stuff to research - this has, and I know I’m gushing a bit, been quite the adventure. I’ll create and upload a picture to make it more clear what I’m trying to do.
Yeah @madworm, that’s what the OSHPark person told me as well - 100mils router for outlines. They also said it was important to add text to the cutout area indicating that it is a cutout to make it easier for the fab to identify.
