Using Kicad 4.0.6 with a 2.54mm Edge-Cuts width with some mouse-bites
I did a simple RJ45 adapter board for various sensors but I have the following issues :
First question, where did you get your mouse-bites? Some have drawings on the edge cuts layer, some don’t. Either way, you need to make sure the outline is a continuous line, otherwise the 3D viewer gets confused. You can ignore the 3D viewer, it’s inconvenient but doesn’t affect the gerbers.
I think there are problems with that site, it didn’t work correctly on some files I uploaded. It’s a neat idea turning the gerbers into a 3D view, I’ve seen one that also displays components.
That looks like a problem with inch/mm conversion, or number of decimals in the gerbers. I am sure we have seen that before, I don’t remember the fix.
It’s discouraged to do slots on the outline layer, by using the thickness of the edge.cuts drawing and create non-closed outlines that way… KiCAD definitely doesn’t like it and freaks out. Your parts will become bigger and clearance setbacks of zones will be affected, as the fab will mill the outline to it’s center, and not it’s ‘internal’ edge. Your slots will barely reach the outline milling and the fab will have extra work to pull the slots out of the edge.cuts layer, if they even accept it (= extra work).
A lot of Gerber viewers don’t like it and will crap out on you.
I think it’s a remnant of similar discouraged stuff, like overlapping drills to create an elongated slot. #Don’t do it.
.
Chose either:
draw slots as outline
like this (usually 0.15 mm edge.cuts line thickness) on a 0.5 mm grid (very easy to get ends to meet):
draw slots on another layer,
like EcoX.User (in the width of the slot) & only draw the outline on the edge.cuts layer and communicate this with your fab be warned though - this won’t get you a 3D view of the slots and will also not work on zones or other stuff during layout, as KiCAD nor freerouters will expect this method for defining ‘no go areas’ on your board
PS: if you do it via the outline method, you don’t have to do the round internal ‘ends’ as the milling bit will take care of that - they usually use the biggest they can get away with that fit’s into your slot. For 1.6 mm pcb a 1 mm min width slot causes no trouble, for 2 mm pcb a 1.5 mm min width slot is advised (always talking center to center of outline here = thickness of the outline doesn’t matter mechancially, only for KiCAD in regards to zone setbacks, which is a bug).
It is also useful to be able to adjust edge keep-out section by section.
But maybe edge line thickness should not be the method as it would look
much better if edge outline has a consistent width regardless of Keep-out
That is something you need to ask your manufacturer. We do not know what their smallest milling tool size is.
This should be listed in their specifications. If not you need to either call them or write an email.
I have 1 mm slots in 1.6 mm pcb all the time with Chinese fabs. No problem so far.
For 2 mm pcb I go up to 1.5 mm slot width, also no complaints.
If it’s a lot of milling they will come back to you and ask for more money, as they can ‘see’ the panels and naturally want to let you in on the milling bit wear and tear cost
The wider your slots are, the less problem you will have, as the bits get bigger and the wear&tear goes down.
All depends on the actual fab you’re going to use.
Only they will know.
With my current design, I was charged 1 base plus 4 extra designs… so I changed all to the left design with edge cuts for v-cuts for middle those in the middle, I ended up not using any mouse bites ( stamp holes ) at all…
Below is the final design I submitted and accepted as 1 design …
