I’m using V5 and created a new foot print with oval holes. When I sent this to my fabricator to check he come back with this.
“I’ve just had a quick look and they come through as drilled slots, which is essentially just a series of holes that all over lap. We do them as a route instead, as the end result is normally cleaner and also doesn’t require special slot tools. Do you get given an option when you define the slots to select between drilled or routed slots?”
Is there a way to define these oval holes as slots?
I suspect not, so I change the footprint to pads on the top and bottom layers of type Connector and then put a slot on one of the user layers. I will then inform the fabricator that this layer is for plated slots. Is there a better way to do this?
There are several options for drill files, which did you use?
When I use the gerber format it has one hole, a slot, not series of drilled holes. Maybe the manufacturer’s CAD->CAM conversion programs make it a series of holes, but I think it’s their problem. On the other hand I don’t know how they are normally handled.
I click Generate Drill File and get *.NPTH.drl and *.PTH.drl files.
Good point about it being the software at their end. When I use Gerbv 2.6.0 to view the drill file the slot just shows as a circular hole. I guess this is going to be manufacture dependent. I have a workable solution for now I think. It’s a bit clunky though.
Oval holes/slots are a regular problem. I think KiCad generates a “drill + drag” method, which could theoretically could be converted by CAM to software a row of drills or a route operation, but generally it seems they either regard it as single hole or an invalid operation.
That means the user has to know the preferences of the manufacturer, and change the footprint accordingly, and also manually add routes since edge cuts are not allowed in footprints . I suppose that KiCad could handle it via a CAM option, but someone will need to write a patch and get it accepted…
Some manufacturers accept edge cuts, routes and v-scores all on the edge cuts layer, some don’t, so it’s a messy thing to deal with.
When I was doing a board with a barrel connector the slots would show up in the Gerbers as holes instead of slots. If I used the experimental Gerber 2 they showed as slots. If they take Gerber 2 format (which I’ve read doesn’t have wide acceptance yet) this might help.
See the post above, this may be a file setting issue.
Also calling the choices
[] excellon
[]gerber X2(experimental)
is a semantic error that should be fixed - Gerber plot files are NOT Excellon, that is a drill file format.
There are actually multiple Gerber choices -
Basic (aperture flash) Gerber goes back decades (60’s), RS-274X is very widespread, (1998) and the X2 is somewhat new.(2014)
KiCad should ideally give a choice of RS-274X. and X2.
If you use both options, how do the files compare ?
. I suppose that KiCad could handle it via a CAM option, but someone will need to write a patch and get it accepted…