I have a capacitor in my schematic . But the footprint of the actual capacitor which i chose is having four pins . How do i connect or take care of these extra pins in my PCB editor ?
Its a little ugly but if you want to make sure that the schematic nets are connected together than you can simply place the symbols pins on top of each other.
That’s what I did for regulator LD1117S33CTR which has a tab that is also connected to the Vout pin.
Or you could set the footprint pad to the same pin number.
Or if they aren’t connect to anything you can set the extra pins in the Schematic symbol to hidden.
I recently had this problem with a 7805 3-terminal regulator in TO-220 package.
I left the schematic symbol in EESCHEMA with only 3 terminals (IN, COMMON, and OUT). Then I created a footprint for PCBNEW that combined two of the package’s physical pins into a single electrical pad. This single electrical pad is actually composed of FOUR overlapping footprint pads:
- A rectangular SMD pad that underlies the entire package body, and extends slightly beyond the package edges (560 x 775 mils). This pad is identified as pad number “2”. I specified “Solid” connections to copper fill zones for this pad, so it becomes the basis for a heatsink.
- A “pad” composed of only a NPTH hole (150 mils - #6 clearance), to receive the component mounting screw. This pad can not be assigned a pad number, which may be the source of the DRC squawk discussed below.
- An oval through-hole pad, 70x140 mils (with 43 mil hole), to receive the TO-220 center pin. This pad is also identified as pad number “2”.
- A rectangular SMD pad (70x730 mils) overlapping and extending through all of the above pads. This one is identified as pad number “2” (surprise!).
The remaining package connections (pad “1” and “3”) are routine through-hole pads.
This footprint works, which can be verified by inspection of Gerber files. (OK, the assemblers may cuss you if they are required to solder the tab, but if you simply screw down the tab and make the electrical connection through the center pin their suffering is significantly reduced.)
UNFORTUNATELY . . . . this footprint throws a DRC squawk: “ErrType(19): Pad near pad”. This seems to be a conflict between the NPTH hole and the large SMD pad for the tab. I’m guessing it’s because the NPTH hole doesn’t have a pad number assigned. (In general, KiCAD allows pads to overlap and have electrical connectivity as long as they have identical pad numbers and the overlap is substantial, not just touching. This seems to be a useful feature for situations like this.)
(My apologies, it took a bit of poking around to figure out how to attach a file.) TO-220_Horiz_ThermalPad.kicad_mod (2.6 KB)
Thank you for the feedback. I also made a new schematic for the capacitor and added corresponding pins in the footprint.