Footprint vs trace

I want to modify this footprint such that the 1 in the center is connected to the 1 cluster.
Is it possible to do it in the footprint? Or is it recommended to use a trace?

Adding traces to footprints is not recommended and can lead to problems, so I would only do it if necessary. Is the purpose to save time when doing layout?

A screenshot would help a lot here.

The original maker used a trace to connect the pads.
But I want to understand the reason why it’s not connected in the footprint instead. Or is it also possible?

KiCad doesn’t support traces in footprints… it’s just the way the code was written. You can hack in graphical shapes into the footprint, but it leads to problems later.

Watch out with that footprint. Not many board houses support overlapping drill hits. (It can easily break a drill bit.) Try using an oval drill hole in those pads.

If you must connect pads within a footprint, try using rectangular SMT pads between THT pads. Note, this will take away any flexibility when laying out the board on what side of the board the connecting trace should be.

1 Like

There might also be the issue of too little copper around the drill. (In the right screenshot at least)

Most manufacturers give a minimum annular ring requirement. @Ahy2pien check if your footprint follows these requirements.

Everyone’s comments here are valid. Watch for overlapping drills and sufficient copper.

Now, if you want to connect the two, you should place another pad (SMD) between the two pins. Remove the mask and paste layers. Then it will behave like a trace. Make sure to give it the same pin number.

See attached for an example.

In KiCad 4.0.7, when I use the attached footprint, it shows
IO_ERROR: PARSE_ERROR: Expecting ‘circle, rectangle, oval, or trapezoid’ in input/source
line 49
offset 14
from dsnlexer.cpp : Expecting() : line 369
from kicad_plugin.cpp : Load() : line 327

Should I use KiCad 5.0? Or is there a plugin?

What will be the problems when I ‘hack’ the SMD pad to connect the pads?

It looks like the footprint @Seth_h designed does use use a rounded rectangle pad. As i assume this is simply an example footprint to showcase how something like this is done it is not necessary to switch to a more experimental version of kicad that still comes with some problems just to do this sort of thing.

Here the same footprint but with the rounded rectangle pad converted to a normal rectangle pad: MX-ALPs-PG1350-FLIP.kicad_mod (5.2 KB)

It does remove options for the layout guy. (As others already stated.) As one normally does not really know how the restrictions are for the layout side while designing the footprint it is not wise to do such a thing.

Thanks @Rene_Poschl ! You are correct on all counts.

There was nothing special about the rounded rectangle, just forgetfulness on my part. And I agree that without a footprint-level requirement such as directionality or minimum connection surface, this hack-y approach is to be avoided.

thank you all!!1 I can open the footprint with a rect pad

when I draw the trace, it shows the upper pads are not connected. How do I solve this in the right way?

The “right” way is to draw a trace between the two pins.

If you want the pad to connect your pins, you will need to overlap the centers of the pins with your pad. See attached for an example (this is with a standard rect). If you want different shapes in 4, you’ll need to add multiple rectangles and overlap them.

MX-ALPs-PG1350-LED-FLIP.kicad_mod (5.4 KB)

I guess I should use a trace instead :slight_smile: thanks everyone

1 Like

when the hole is ø1.2mm, what’s the recommended minimum copper pad size?

Depends on your manufacturer. Look up their design requirements. (look for minimum annular ring.)

If there is no annular ring listed you will need to use their tolerance information to arrive at the value (drill tolerance, alignment tolerances, tolerances for copper features)

According to IPC it should be at least 0.15mm So 1.2+2*0.15mm

The footprint shared by @Seth_h and reworked by me seems to be ok in this regard.