Nothing fancy, but I would like to route a wire starting from some pin above pin 9, and going between
9 and 7, then 10 and 8 in an internal layer (I’m working on a 4 layer PCB). The problem is that the router
(manual) refuses to draw a trace between 10 and 8, it goes around the connector. I’'m not sure about the
size of the holes, but that may be the problem. I use a wire width of 0.125, which is the standard with
my PCB maker. I could of course set it to 0.1, but the cost would increase.
Are the internal hole pads similar in size? In Eagle, there was a separate description of internal and
external layers rules. Is there such a differenciation in Kicad?
How can I solve this without redefining custom footprints?
Kicad is probably refusing to make the connection between Pin 8 and Pin 10 because Pin 8 and Pin 10 do not belong to the same net. On your schematic, verify that there is truly a connection between Pin 8 and Pin 10, and not an almost-but-not-quite connection that falls short by a few pixels.
hermit > I believe the yellow circle is the clearance tolerance.
Ok, I thought the yellow part was a symbol of the rest ring. But thanks, it was a very good hint.
Anyway, I did something, and in case it can be of some help to somebody, here is what I did:
Double-clicking one particular pad (I mean hole) in the picture I attached in the first mail, brings some panel allowing me to change a few things. As a reminder, I’m using a 1.27 mm pitch IDE connector and I want to draw a 0.125 wire between 2 holes (without touching them, and staying at the right distance of each of them. The right distance, the clearance is at least 0.125 for my PCB maker, same as the wire. Therefore the holes have to be separated by at least 0.375 mm, therefore the pads have to be at most (1.27 - 3*0.125) = 0.895mm in diameter. I will set them at 0.85 so that it works even if Kicad has some rounding issues.
After correcting the diameters, select the pad you just edited, right click and open “pad” which is the last item of the context menu.
In the Pad menu, choose “push pad properties”. A popup window is displayed. Choose "change pads on footprint:, and all the pads of the current footprint will be altered.
The following picture shows the results. As you can see, I can now draw one wire between pads.
My guess is that the yellow circle (the line only circle) represents the resulting pad clearances.
Clearance can be set on 3 places (lowest priority to highest)
Project wide (set this to the board manufacturer specification. Or a bit above it)
Footprint wide (every footprint can overwrite the project setting. Use this to either force a different clearance for a full footprint. Often used for critical parts like BGAs)
Per pad (ever pad can define its own clearances. This is used if you want tight control over a particular pad)
The violet filled cirlce might represent the mask cutout. Mask cutouts should always be smaller than clearance to avoid having nearby traces without mask coverage.
Thanks for your reply. I didin’t notice and could manage to do something, but anyway your explanation of
the 3 level setup will certainly become useful at some point.
By the way, I just understood which “yellow circle” in Hermit’s reply.
