kicad-developers team mailing list archive

[Tomasz Wlostowski <tomasz.wlostowski@xxxxxxx>]

On 08.06.2015 12:24, Cirilo Bernardo wrote:
> One method which comes to mind is to add yet another hole definition in
> software, and that may be the best way to address the problem; this way
> we can also ensure the correct thickness of the annulus and check the
> chosen number/size of vias.

There is another way: don't use a pad to simulate a via. Letting vias
retain their nets (or - in case of footprints - follow the connectivity
starting from pads) is IMHO a way to fix this and many other issues
(thermal via fields, etc.)

Tom
> 
> - Cirilo
> 
> 
> On Mon, Jun 8, 2015 at 5:59 PM, Lorenzo Marcantonio
> <l.marcantonio@xxxxxxxxxxxx <mailto:l.marcantonio@xxxxxxxxxxxx>> wrote:
> 
>     Having troubles getting an useable workflow with a common usage: the
>     mounting
>     hole with satellite vias (see attachment).
> 
>     Rationale: when you have a big hole for a screw and need to have plane
>     connectivity, a PTH supported pad is often not a good choice. Mostly
>     because on
>     the wave solder machine they tend to get clogged (requiring an
>     expensive peel
>     mask). There are other reason, like ground plane impedance, but
>     manufacturing
>     convenience is the biggest one :P
> 
>     So I did the following thing:
> 
>     (module "HOLE-M4-NPTH" (layer "F.Cu") (tedit 557548BB)
>             (descr "Mechanical Hole, M4")
>             (attr virtual)
>             (fp_text reference "HOLE-M4-NPTH" (at 0 0) (layer "F.Fab")
>                      (effects (font (size 1.2 1.2) (thickness 0.12))))
>             (fp_text value "HOLE-M4-NPTH" (at 0 0) (layer "F.Fab") hide
>                      (effects (font (size 1.2 1.2) (thickness 0.12))))
>             (fp_circle (center 0 0) (end 5.85 0) (layer "F.CrtYd")
>     (width 0.01))
>             (fp_circle (center 0 0) (end 5.85 0) (layer "B.CrtYd")
>     (width 0.01))
>             (fp_circle (center 0 0) (end 5.5 0) (layer "F.SilkS") (width
>     0.12))
>             (fp_circle (center 0 0) (end 2.2 0) (layer "F.Fab") (width
>     0.12))
>             (fp_circle (center 0 0) (end 2.2 0) (layer "B.Fab") (width
>     0.12))
>             (fp_circle (center 0 0) (end 2.2 0) (layer "Dwgs.User")
>     (width 0.12))
>             (pad "" np_thru_hole circle (at 0 0) (size 4.4 4.4) (drill
>     4.4) (layers "*.Cu"))
>             (pad "HOLE" smd circle (at 0 0) (size 8.35 8.35) (layers
>     "*.Cu"))
>             (pad "HOLE" thru_hole circle (at 3.2 0) (size 0.8 0.8)
>     (drill 0.4) (layers "*.Cu")
>                  (zone_connect 2))
>             (pad "HOLE" thru_hole circle (at -3.2 0) (size 0.8 0.8)
>     (drill 0.4) (layers "*.Cu")
>                  (zone_connect 2))
>             (pad "HOLE" thru_hole circle (at 1.6 -2.8) (size 0.8 0.8)
>     (drill 0.4) (layers "*.Cu")
>                  (zone_connect 2))
>             (pad "HOLE" thru_hole circle (at -1.6 -2.8) (size 0.8 0.8)
>     (drill 0.4) (layers "*.Cu")
>                  (zone_connect 2))
>             (pad "HOLE" thru_hole circle (at -1.6 2.8) (size 0.8 0.8)
>     (drill 0.4) (layers "*.Cu")
>                  (zone_connect 2))
>             (pad "HOLE" thru_hole circle (at 1.6 2.8) (size 0.8 0.8)
>     (drill 0.4) (layers "*.Cu")
>                  (zone_connect 2)))
> 
>     I have a big SMD round pad on all layers for the support copper, an
>     NPTH hole
>     for the drill tape, and common pads for the satellite vias. The
>     zone_connect forces solid fill, not that it would have really mattered
>     (since there is the big pad covering all). Less cruft in the gerbers...
> 
>     Problem #1: pad snap always pick the big SMD pad and the track get
>     rejected because it falls into the NPTH hole; workaround: disable pad
>     snap and locate it by hands. Not a big issue since usually these are
>     tied to fills and they attach correctly.
> 
>     Problem #2: the big pad and the NPTH hole are conflicting in the DRC
>     (quite correctly, in theory). However that's a PITA because the message
>     can 'obscure' more severe errors.
> 
>     Any idea on how to solve this?
> 
>     --
>     Lorenzo Marcantonio
>     Logos Srl
> 
>     _______________________________________________
>     Mailing list: https://launchpad.net/~kicad-developers
>     Post to     : kicad-developers@xxxxxxxxxxxxxxxxxxx
>     <mailto:kicad-developers@xxxxxxxxxxxxxxxxxxx>
>     Unsubscribe : https://launchpad.net/~kicad-developers
>     More help   : https://help.launchpad.net/ListHelp
> 
> 
> 
> 
> _______________________________________________
> 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
>