Re: [Kicad-developers] How to handle mounting holes with satellite vias?
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.marcanto...@logossrl.com mailto:l.marcanto...@logossrl.com 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@lists.launchpad.net mailto:kicad-developers@lists.launchpad.net Unsubscribe : https://launchpad.net/~kicad-developers More help : https://help.launchpad.net/ListHelp ___ Mailing list: https://launchpad.net/~kicad-developers Post to : kicad-developers@lists.launchpad.net Unsubscribe : https://launchpad.net/~kicad-developers More help : https://help.launchpad.net/ListHelp ___ Mailing list: https://launchpad.net/~kicad-developers Post to : kicad-developers@lists.launchpad.net Unsubscribe : https://launchpad.net/~kicad-developers More help : https://help.launchpad.net/ListHelp
Re: [Kicad-developers] How to handle mounting holes with satellite vias?
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. - Cirilo On Mon, Jun 8, 2015 at 5:59 PM, Lorenzo Marcantonio l.marcanto...@logossrl.com 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@lists.launchpad.net Unsubscribe : https://launchpad.net/~kicad-developers More help : https://help.launchpad.net/ListHelp ___ Mailing list: https://launchpad.net/~kicad-developers Post to : kicad-developers@lists.launchpad.net Unsubscribe : https://launchpad.net/~kicad-developers More help : https://help.launchpad.net/ListHelp
Re: [Kicad-developers] How to handle mounting holes with satellite vias?
On Mon, Jun 08, 2015 at 01:15:39PM +0200, Tomasz Wlostowski wrote: 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.) The main problem is another way: the NPTH conflicts with the main pad; I don't really care about the vias (since they don't harm DRC) Maybe special-casing hole in the same module could be a solution, if you trust people do to correct modules... -- Lorenzo Marcantonio Logos Srl ___ Mailing list: https://launchpad.net/~kicad-developers Post to : kicad-developers@lists.launchpad.net Unsubscribe : https://launchpad.net/~kicad-developers More help : https://help.launchpad.net/ListHelp
Re: [Kicad-developers] How to handle mounting holes with satellite vias?
In response to a message written on 08.06.2015, 14:37, from Lorenzo Marcantonio: On Mon, Jun 08, 2015 at 01:15:39PM +0200, Tomasz Wlostowski wrote: 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.) The main problem is another way: the NPTH conflicts with the main pad; I don't really care about the vias (since they don't harm DRC) Maybe special-casing hole in the same module could be a solution, if you trust people do to correct modules... IMHO, there is no any obstacles, that NPTH pads can have some net, only last wall is in peoples minds… ;) -- Best Regards, LordBlick ___ Mailing list: https://launchpad.net/~kicad-developers Post to : kicad-developers@lists.launchpad.net Unsubscribe : https://launchpad.net/~kicad-developers More help : https://help.launchpad.net/ListHelp
Re: [Kicad-developers] How to handle mounting holes with satellite vias?
On Mon, Jun 08, 2015 at 02:57:46PM +0200, LordBlick wrote: IMHO, there is no any obstacles, that NPTH pads can have some net, only last wall is in peoples minds… ;) There *are* issues having a net attached to an NPTH, at least last time I checked (i.e. when they where added). pcbnew has no handling for holes which don't connect planes, that's the biggest one :D At the time I pondered a lot about it and I were with the 'no net to NPTH pads' peoples. -- Lorenzo Marcantonio Logos Srl ___ Mailing list: https://launchpad.net/~kicad-developers Post to : kicad-developers@lists.launchpad.net Unsubscribe : https://launchpad.net/~kicad-developers More help : https://help.launchpad.net/ListHelp
Re: [Kicad-developers] How to handle mounting holes with satellite vias?
I use this workaround ... I manually added net number to the NPTH drill pad (with notepad)... please find attached the pcb module then you can use this module inside a library (import without editing and save lib) and it is possible to wire tracks and there is no DRC violations... maybe to solve this prob in a clean way it could be nice to add the option to have pin nbr also for NPTH drill pad... Regards Maurice On 08/06/2015 14.37, Lorenzo Marcantonio wrote: On Mon, Jun 08, 2015 at 01:15:39PM +0200, Tomasz Wlostowski wrote: 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.) The main problem is another way: the NPTH conflicts with the main pad; I don't really care about the vias (since they don't harm DRC) Maybe special-casing hole in the same module could be a solution, if you trust people do to correct modules... (module a_ANCHORS:1pinD35-NPTH-drilled (layer F.Cu) (tedit 55758F44) (fp_text reference J*** (at 0 -4.699) (layer F.SilkS) hide (effects (font (size 1.00076 1.00076) (thickness 0.2032))) ) (fp_text value anchor (at 0 4.953) (layer F.SilkS) hide (effects (font (size 1.00076 1.00076) (thickness 0.2032))) ) (fp_circle (center 0 0) (end 0 1.6764) (layer B.SilkS) (width 0.16)) (fp_circle (center 0 0) (end -0.0254 1.6764) (layer F.SilkS) (width 0.16)) (fp_circle (center 0 0) (end 0 3.556) (layer B.SilkS) (width 0.16)) (fp_circle (center 0 0) (end 0 3.556) (layer F.SilkS) (width 0.16)) (pad 1 thru_hole circle (at 0 -2.2606) (size 0.6 0.6) (drill 0.381) (layers *.Cu *.Mask)) (pad 1 thru_hole circle (at -2.2606 0) (size 0.6 0.6) (drill 0.381) (layers *.Cu *.Mask)) (pad 1 thru_hole circle (at 0 2.2606) (size 0.6 0.6) (drill 0.381) (layers *.Cu *.Mask)) (pad 1 thru_hole circle (at 2.2606 0) (size 0.6 0.6) (drill 0.381) (layers *.Cu *.Mask)) (pad 1 thru_hole circle (at 1.6002 -1.6002) (size 0.6 0.6) (drill 0.381) (layers *.Cu *.Mask)) (pad 1 thru_hole circle (at -1.6002 -1.6002) (size 0.6 0.6) (drill 0.381) (layers *.Cu *.Mask)) (pad 1 thru_hole circle (at -1.6002 1.6002) (size 0.6 0.6) (drill 0.381) (layers *.Cu *.Mask)) (pad 1 thru_hole circle (at 1.6002 1.6002) (size 0.6 0.6) (drill 0.381) (layers *.Cu *.Mask)) (pad 1 np_thru_hole circle (at 0 0) (size 3.5 3.5) (drill 3.5) (layers *.Cu *.Mask F.SilkS)) (pad 1 smd circle (at 0 0) (size 5.6 5.6) (layers F.Cu F.SilkS F.Mask)) (pad 1 smd circle (at 0 0) (size 5.6 5.6) (layers B.Cu B.SilkS B.Mask)) ) ___ Mailing list: https://launchpad.net/~kicad-developers Post to : kicad-developers@lists.launchpad.net Unsubscribe : https://launchpad.net/~kicad-developers More help : https://help.launchpad.net/ListHelp
