kicad-developers team mailing list archive

[Seth Hillbrand <seth@xxxxxxxxxxxxx>]

Hi Steven-

If you would like to create your own jumper pads that don't fail DRC, you
have a couple of options.

1) Create a graphic polygon on the copper layer of the footprint (see
attached image).  To do this, you need to create the graphic polygon in the
footprint editor and then edit it to move it to the F.Cu layer.  You will
get a warning that this is dangerous because it is not handled by DRC.
This is both accurate and what you want.  Note that this is a non-supported
option and may be removed or changed in the future.  The reason it passes
DRC is that DRC doesn't check whether there are issues.  It may also cause
issues with zone fills depending on your settings.

2) Change the symbol in the library editor to have both pins share the same
pin number (1).  Then, change the footprint to have all pads be number
"1".  This is not technically a net tie anymore as it just joins the nets
together into a single net but it is effectively the same as your image.

Do feel free to add your input to this bug report:
https://bugs.launchpad.net/kicad/+bug/1571930

Best-
Seth



Am Mi., 11. Juli 2018 um 05:46 Uhr schrieb Strontium <strntydog@xxxxxxxxx>:

> So,
>
> I tried to use the PCB Jumpers from the standard library, specifically a
> NC jumper. Jumper:SolderJumper-2_P1.3mm_Bridged_RoundedPad1.0x1.5mm
> These seem to be new with the V5 library, because i don't remember them
> with V4.
>
> And it causes DRC errors.  Firstly it generates "Track near Pad" DRC
> errors, because its built from overlapping pads, and specifically the
> middle pad used to create the NC connection is too close to the track
> which terminates on the "Actual" pads.
>
> So i made a local change to eliminate that by reducing the size of the
> "joining" pad.  But that still causes a DRC error "Pad near Pad", which
> is right, because its just a bunch of overlapping pads.  So the question
> is, How is one supposed to use this standard library component without
> generating DRC errors.
>
> I tried a bunch of experiments to create a NC Solder Jumper that doesn't
> create DRC errors and the best workaround seems to be use a NO PCB
> Jumper and manually connect the pins in the schematic like this:
>
> https://imgur.com/a/HwXKttp
>
> Which works, and doesn't generate DRC errors, because I have to manually
> connect the pads with a fat track, DRC passes.  BUT it is ugly from a
> schematic perspective.
>
> It seems like there needs to be a copper feature of a footprint, that is
> not a PAD (or at least is ignored for PAD DRC checks) to handle cases
> like this.
>
> Don't get me wrong because i think the Solder Jumper components look
> great, but should there be standard components that can't pass DRC?
>
> Steven
>
>
>
> _______________________________________________
> Mailing list: https://launchpad.net/~kicad-developers
> Post to     : kicad-developers@xxxxxxxxxxxxxxxxxxx
> Unsubscribe : https://launchpad.net/~kicad-developers
> More help   : https://help.launchpad.net/ListHelp
>

Attachment: Screenshot_2018-07-11_10-59-04.png
Description: PNG image