Unplated holes to drill file

[Jaanus-kalde]

It would be nice to have some way of making non plated holes to NC drill file. In eagle it is done with marking it with a drill hole but taking all the copper away from board, and all the board houses accept this.

At the moment I'm making mechanical drill holes with equal size and drill. Then manually deleting copper from the insides of the drillholes. Or drawing the holes on Edge Cuts layer with circles. Both are workarounds to a problem that shouldn't be there.

It is weird that there is about 4 ways to make mechanical holes but still no normal way that is acceptable by board houses.

Linux mint 12
Build:(2013-feb-21)-testing

[Lorenzo Marcantonio (l-marcantonio)]

On Tue, Feb 26, 2013 at 02:32:44PM -0000, Jaanus-kalde wrote:
> Public bug reported:
>
> It would be nice to have some way of making non plated holes to NC drill
> file. In eagle it is done with marking it with a drill hole but taking
> all the copper away from board, and all the board houses accept this.
>
> At the moment I'm making mechanical drill holes with equal size and
> drill. Then manually deleting copper from the insides of the drillholes.

Choose mechanical hole in the pad properties, another drill tape will be
generated with unplated holes. If you don't have that choice, upgrade
pcbnew :D

--
Lorenzo Marcantonio
Logos Srl

[Dick Hollenbeck (dickelbeck)]

Each bug report must be accompanied with the version of the software that is being reported, and the operating system.

[Jaanus-kalde (jaanus-kalde)]

Yes, I know about mechanical drill holes, but these generate two drill files and I have not seen any board house that accepts two drill files as a default.

[Lorenzo Marcantonio (l-marcantonio)]

On Tue, Feb 26, 2013 at 03:40:46PM -0000, Jaanus-kalde wrote:
> Yes, I know about mechanical drill holes, but these generate two drill
> files and I have not seen any board house that accepts two drill files
> as a default.

OK, then it would be wishlist for a merged drill file.

I agree it would be useful, some fabricator are picky on these...

--
Lorenzo Marcantonio
Logos Srl

[Wayne Stambaugh (stambaughw)]

I'm aware of this issue myself as some PCB vendors is use prefer a single drill file containing both plated and non-plated though holes and merging them by hand is less than ideal. Someone recently submitted a patch on the mailing to resolve this issue but it needed some work before it can be committed. If I don't here back from the original patch author, I will go ahead an make the change myself.

[Martin Errenst (imp-d)]

The mentioned mail with the original patch is: https://lists.launchpad.net/kicad-developers/msg09331.html .
Made the changes with wxformbuilder, fixed some code style issues. Applies with the current revision (r4729). Please credit Matthew Lai for this patch :).

[jean-pierre charras (jp-charras)]

Before changing the current Kicad behavior, I need to know what some official document (something like an IPC standard or some other document) said about this.
Otherwise, we need to write a new feature or option for each board manufacturer in the world.

[Wayne Stambaugh (stambaughw)]

On 2/28/2014 7:22 PM, Martin Janitschke wrote:
> The mentioned mail with the original patch is: https://lists.launchpad.net/kicad-developers/msg09331.html .
> Made the changes with wxformbuilder, fixed some code style issues. Applies with the current revision (r4729). Please credit Matthew Lai for this patch :).
>
> ** Patch added: "adds option to merge drillfiles on export"
> https://bugs.launchpad.net/kicad/+bug/1133330/+attachment/4001595/+files/merge-drill-files-option.patch
>
> ** Changed in: kicad
> Status: Incomplete => Confirmed
>
Patch fails to build against product branch revision r4731 with
following error:

e:/src/kicad-testing/trunk/pcbnew/exporters/gen_drill_report_files.cpp:
In membe
r function 'bool EXCELLON_WRITER::GenDrillReportFile(const wxString&)':
e:/src/kicad-testing/trunk/pcbnew/exporters/gen_drill_report_files.cpp:363:76:
e
rror: no matching function for call to
'EXCELLON_WRITER::BuildHolesList(LAYER_NU
M&, LAYER_NUM&, bool, bool&)'
e:/src/kicad-testing/trunk/pcbnew/exporters/gen_drill_report_files.cpp:363:76:
n
ote: candidate is:
In file included from
e:/src/kicad-testing/trunk/pcbnew/exporters/gen_drill_repo
rt_files.cpp:43:0:
e:/src/kicad-testing/trunk/pcbnew/exporters/gendrill_Excellon_writer.h:203:10:
n
ote: void EXCELLON_WRITER::BuildHolesList(int, int, bool, bool, bool)
e:/src/kicad-testing/trunk/pcbnew/exporters/gendrill_Excellon_writer.h:203:10:
n
ote: candidate expects 5 arguments, 4 provided
make[2]: ***
[pcbnew/CMakeFiles/pcbnew.dir/exporters/gen_drill_report_files.cpp.
obj] Error 1
make[1]: *** [pcbnew/CMakeFiles/pcbnew.dir/all] Error 2
make: *** [all] Error 2

[Martin Errenst (imp-d)]

Fixed this (surprised that this slipped through...).
JP there are standards and there are industry /standards/ not following the first ones ;/.

[jean-pierre charras (jp-charras)]

I am thinking this is not a "industry /standards/":
My board house wants 2 separate files.

Some footprints need a mechanical hole with copper around the hole (components like very small leds or photo-detectors which are in fact inside the hole)

And trust me, "industry /standards/" is very country dependent.

However I did not asked for an "official standard",
but just only any serious document about this (surprised that this slipped through...).

[Chris Gibson (chris-w-gibson)]

I agree with JP.

We use two different board houses. One likes a single file. The other likes two separate files (both in UK).

[Martin Errenst (imp-d)]

See https://bugs.launchpad.net/kicad/+bug/1281786 (the initial post), they want an merged drill file for example.

[Martin Errenst (imp-d)]

Regarding those components with the unplated holes with copper (direct up to the hole? Does it make problems later due to the missing pull back??), they will be broken by those fabs i guess, unless you specify a small pullback around those holes...
All the fabs I've used took two different files, and that's fine imho. Due to the fact that I suspect that oshpark might be quite popular in some parts of the community and the same request appearing twice in the bug tracker (and Chris confirming that there are even more doing this), it's worth adding this function to KiCad. It doesn't hurt and it's not a new fancy format for export that will later need much care while moving on :).

[Daniel Holth (dholth)]

For what it's worth there is at least one other fab that likes getting a
single drill file. http://forum.iteadstudio.com/viewtopic.php?f=14&t=699

I think it has to do with differences in how the NPTH are manufactured.
Some fabricators can drill both plated and unplated holes in a single
step. Then the unplated holes are covered with a mask, the board is
plated, and later the mask is dissolved. Citation needed. Others drill
the NPTH last. So it is possible that the preferred number of drill
files corresponds to the number of manufacturing steps used by a
particular fab.

On Mon, Mar 3, 2014, at 09:01 AM, Martin Janitschke wrote:
> Regarding those components with the unplated holes with copper (direct up
> to the hole? Does it make problems later due to the missing pull back??),
> they will be broken by those fabs i guess, unless you specify a small
> pullback around those holes...
> All the fabs I've used took two different files, and that's fine imho.
> Due to the fact that I suspect that oshpark might be quite popular in
> some parts of the community and the same request appearing twice in the
> bug tracker (and Chris confirming that there are even more doing this),
> it's worth adding this function to KiCad. It doesn't hurt and it's not a
> new fancy format for export that will later need much care while moving
> on :).
>
> --
> You received this bug notification because you are subscribed to a
> duplicate bug report (1281786).
> https://bugs.launchpad.net/bugs/1133330
>
> Title:
> Unplated holes to drill file
>
> To manage notifications about this bug go to:
> https://bugs.launchpad.net/kicad/+bug/1133330/+subscriptions

[Wayne Stambaugh (stambaughw)]

Patch committed in product branch version r4732. Thanks Martin.

[m (easyw)]

Hi,
as asked at the forum:
https://forum.kicad.info/t/creating-a-footprint-with-drilled-holes/1625/13
some people need a merged drill file for e.g. OSHpark and Itead fabs
It would be nice to have the option to merge them again, as in previous versions...
and following a link where users are talking about this issue:
http://electronics.stackexchange.com/questions/78094/how-to-specify-castellations-in-gerber-files
'So a 'standard' way of defining this is just to have copper over the edges of your castellations. This is how vias and plated through holes work - and conversely, this is how non-plated holes work as well (you just pull back the copper a little bit from the hole). '
Maurice

[Wayne Stambaugh (stambaughw)]

Please do not change the bug report status. This is the job of the bug
managers. The fix for the original bug report was released. You should
create a new bug report.

On 11/11/2015 10:28 AM, m wrote:
> Hi,
> as asked at the forum:
> https://forum.kicad.info/t/creating-a-footprint-with-drilled-holes/1625/13
> some people need a merged drill file for e.g. OSHpark and Itead fabs
> It would be nice to have the option to merge them again, as in previous versions...
> and following a link where users are talking about this issue:
> http://electronics.stackexchange.com/questions/78094/how-to-specify-castellations-in-gerber-files
> 'So a 'standard' way of defining this is just to have copper over the edges of your castellations. This is how vias and plated through holes work - and conversely, this is how non-plated holes work as well (you just pull back the copper a little bit from the hole). '
> Maurice
>
> ** Changed in: kicad
> Status: Fix Released => Opinion
>

[m (easyw)]

ok, sorry...
I rearranged the status and added a new bug @ https://bugs.launchpad.net/kicad/+bug/1515426