DRC doesn't check for overlapping drill holes.

[Agent24]

Running KiCad v 2010-05-05 BZR 2356 -stable

Managed to create a via that was overlapping a pad, without error message.

I have attached the board file. The problem is next to R3 (by the PLCC32 socket)

[Agent24 (tda7000)]

Just to add, this is not such a problem from an electrical point of view since both pad and via are on the same net.

But since I am able to create a via and pad with overlapping drill holes... I don't think any PCB fab places are going to like it very much.

[Lorenzo Marcantonio (l-marcantonio)]

On Fri, 17 Dec 2010, Agent24 wrote:

> Just to add, this is not such a problem from an electrical point of view
> since both pad and via are on the same net.
>
> But since I am able to create a via and pad with overlapping drill
> holes... I don't think any PCB fab places are going to like it very
> much.

Overlapping drill holes are bad, indeed :D

But vias on pad are not (for example thermal vias). Of course you have
to handle solder wicking and suck things.

A 'tented via' option would be useful for them (forcing solder mask on
the via)

--
Lorenzo Marcantonio
Logos Srl

[Martin Errenst (imp-d)]

The DRC still doesn't complain about vias overlapping pads. Also the DRC is totally fine with vias violating each others clearance circle, even with overlapping drill holes - added this case to the boardfile too.
See attached board (reduced from the one above and converted into the new format).

Maybe we can put the test for pad-near-pad into place for via-pad and via-via relation?

Application: Pcbnew
Version: (2014-02-22 BZR 4714)-product Release build
wxWidgets: Version 3.0.0 (debug,wchar_t,compiler with C++ ABI 1002,GCC 4.7.3,wx containers,compatible with 2.8)
Platform: Linux 3.9.2-gentoo x86_64, 64 bit, Little endian, wxGTK
Boost version: 1.54.0
         USE_WX_GRAPHICS_CONTEXT=OFF
         USE_WX_OVERLAY=OFF
         KICAD_SCRIPTING=OFF
         KICAD_SCRIPTING_MODULES=OFF
         KICAD_SCRIPTING_WXPYTHON=OFF
         USE_FP_LIB_TABLE=HARD_CODED_ON
         BUILD_GITHUB_PLUGIN=OFF

[Jeff Young (jeyjey)]

As long as they're the same net, there's nothing to be said about them overlapping.

However, overlapping drill holes should be reported, as they tend to break drill bits.

[Nick Østergaard (nickoe)]

I guess we should also consider pads that are sometimes used where the drills overlap. This is sometimes used over real slots. Just food for thought.

[Jeff Young (jeyjey)]

@Nick, I think most board manufacturers frown heavily on that (carbide drill bits are both brittle and expensive). If people really do need to still do this, then we probably need to put a checkbox in the DRC dialog.

My implementation of the DRC check can be found in my 6.0 tree:

https://git.launchpad.net/~jeyjey/kicad/commit/?h=6.0&id=4faf48508bbb1eecc58c82d8cc5e6e890c235761

[jean-pierre charras (jp-charras)]

One can also just set the min dist to 0 to disable DRC check.

About overlapping holes, although I never used a CAM tool, I am guessing any CAM tool can detect this case, and uses routing bits instead of drilling bits, like in making a slot.
(I think this is a very basic CAM feature to detect if a routing bit must be used: not only for overlapping holes, but also for large sizes: I am guessing a 20mm hole is not created by a 20mm carbide drill bit)