merge plated and unplated drill holes

[m]

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

[jean-pierre charras (jp-charras)]

What I *need* to know is how the board maker recognize the not platted holes.
The basic purpose of 2 files is to recognize plated holes and not platted holes.

[m (easyw)]

I know why KiCad creates correctly two files, but some fabs don't accept two drill files...
OSHPark, which is used by many kicad users, has this rule / way to elaborate NPTH and PTH
"We support both vias (plated holes) and unplated holes. The fab uses the presence of copper underneath the drill hit to determine plating. Copper underneath the drill indicates a via/plated hole, no copper indicates an unplated hole. "
http://support.oshpark.com/support/solutions/articles/107580-drill-specs-settings-and-file
They also suggest to use GerbV from GEDA to merge files, but:
- GerbV doesn't support oval drill
- Why should I use an external tool to merge what kicad could do itself
Moreover I agree with you that this option is a bad habit, but having the option to merge the files (may be with a note that is not the best way to produce drill files) will let OSHPark and other fabs users to produce their boards
When they have a single merged file, they can also add some text info to explain to the fab about the drills....
having just two files will stop them

[espitall (damien-espitallier)]

For your information, Alitum Designer (15.1) default setting is to use only one file. It add ";TYPE=PLATED" or ";TYPE=NON_PLATED" before the tool definition list of each kind.

Example of a single drill file (generated by Altium) with one plated hole and two non_plated holes (with different size) :

M48
;Layer_Color=9474304
;FILE_FORMAT=2:5
INCH,LZ
;TYPE=PLATED
T1F00S00C0.02800
;TYPE=NON_PLATED
T2F00S00C0.02800
T3F00S00C0.03200
%
T01
X017Y025
T02
X016Y027
T03
X018Y027
M30

I have not access to other CAD software, but at least it gives you one way to define the drill type.

[jean-pierre charras (jp-charras)]

Thanks for you info.

[Wayne Stambaugh (stambaughw)]

How many other EDA packages add these comments to their drill files? I
would be reluctant to add board house specific or other EDA specific
comments into our drill files without some serious thought into how we
implement them. I could see this spiraling out of control fairly
quickly as every one will what their own custom comments. I never had
any issues with my board vender (Advanced Circuits) with our old merged
drill file format so I'm fine if we resurrect that. Anything more than
that should be thoroughly researched and discussed.

On 11/13/2015 2:55 PM, jean-pierre charras wrote:
> Thanks for you info.
>

[espitall (damien-espitallier)]

Each EDA have its own comments. Even worse, if I remember correctly Orcad use comment to define hole size (I do not have acces to Orcad to check)

If you provide only one drill file most of board venders will use the copper layer to choose between plated and non-plated. Comments are just a way to not loose informations that can't be implemented because of limitation of the standard.

[espitall (damien-espitallier)]

-- Additional informations --

I have asked a friend who works with PADS (mentor graphics). Default setting is to generate two files. On "one file mode" the software merge the two lists but do not place any information about plated or not.

[m (easyw)]

thank you for the feedback...
I think it would be very useful to have the option to merge the two files as it was
as you pointed out
"If you provide only one drill file most of board venders will use the copper layer to choose between plated and non-plated."

[m (easyw)]

it has been resurrected :)
http://bazaar.launchpad.net/~kicad-product-committers/kicad/product/revision/6317