I made a new footprint in which there is a T shaped pad. I made this pad by setting a regular
pad 2, then drawing a shape on the silk layer, and then use the menu “make pad with selected
items” or something like that. Apparently it worked, and the silk color was instantly converted to
something that looks like copper, red on the top level.
Now my problem is that the pad doesn’t connect to ground copper pour. It works for any other
chip. I have looked at similar questions, but it doesn’t solve my problem.
Note that if I have regular pads, they connect nicely to the ground copper.
In the attached picture, you can notice that there are ratsnest connecting to the nearest chip
ground, but no connections.
Did you use a custom pad? Is it possible that you set its zone connect parameter to none? (I fear this is the default)
This is set in the pad settings dialog (shortcut e or in the right click context menu)
The reason for this is that kicad does not (yet) support automatic thermal relieve for custom pads. As kicads default setting is to use thermals it was decided to make none the default. https://bugs.launchpad.net/kicad/+bug/1732720
If you want thermal relieve for the pad then you can manually add a number of traces connecting it to the copper plane and keep it as zone connect none. Otherwise set the pad to solid connection.
Sounds like you built a custom pad shape, and there is a known issue around thermals on those.
See No ground plane connection on component ground
& bug reports etc.
Note the suggested edge-trim future feature that solves one example, does not solve your case.
The suggestion I made of using the Anchor Pad XYD, would work in your case (but that needs a bug fix).
Your choices are to either manually route short traces, or you can craft that pad shape with two rectangles, both tagged Pin2 (thereby avoiding the Custom Pad issues)
I’m always surprised how fast you reply. I didn’t even have time to finish my coffee.
And in the meantime there is another reply! Than you PCB_Wiz!
Now for this reply:
“If you want thermal relieve for the pad then you can manually add a number of traces connecting it to the copper plane and keep it as zone connect none. Otherwise set the pad to solid connection.”
Keep it as zone connect none: it means that I do nothing special, right?
Set the pad to solid connection: is it a setting in the library? I don’t find anything in the pad properties.
From PCB_Wiz: Your choices are to either manually route short traces, or you can craft that pad shape with two rectangles, both tagged Pin2 (thereby avoiding the Custom Pad issues)
OK, I did it, but the changes in the library are not reflected in the PCB. I tried to set again the footprint from
the schematic, and then re export the schematic, but it doesn’t change anything. By the way, do the 2 rectangles
have to be overlapped? I guess it doesn’t matter, but just in case…
Your choice. If they overlap such that one centre is included, I think that connects automatically, so saves a unconnect report. If they are not touching at all, all pin 2’s rats-nest connect to the same net.
That’s because it already has a footprint imported.
You need to select the footprint and either use change part, or update from library, depending on if you renamed when you changed the method.
