Yes and no. A key advantage of the Perl Script, is you can avoid any other CAD tool, and use only Illustrator.
I would still need to open the output files in something to verify that they are usable.
True, but there are plenty of Gerber Viewers out there.
KiCad has a reasonable one, which can also export to KiCad.
I'll check how that handles Drill....
Addit: Hmm.... well, that
does do Gerber -> KiCad, with some caveats....
* PCB traces come in ok on a per-layer basis
* You can export Drill info to a user layer, so you can see holes and slots
* It seems to sense trace ends, and export as VIA, with a round diameter == Pad length. Drill is always 0.4mm
Caveats:
-- Vias
do have drill (0.4mm), but alas
not derived from the Drill-imported
-- Vias are placed on all PADS, including SMD ones.
-- KiCad Vias I think cannot change from Round, nor manually set Drill = 0.0, or separate layer stack-ups.
I guess that means for a Thru hole PCB, with no SMD, and only round pads, this could work.
One weird thing is slotted oval holes at 45' (ie the most complex) seem to convert ok, but the simpler SMD pads all morph to round ?!
Ahh.. seems flashed items are treated specially, different from drawn.
Flashed to F.Cu or B.Cu flip to Vias, Flashed to drawing layers flip to Round == H Value of Flash, no drill.
With the DXF-import method I'm not using other CAD tools for anything other than compiling the PCB layers and generating the Gerber files. Well, ideally that's the case anyway. As it stands, DipTrace won't accept imported DXF drill holes so I have to add those from within the program. I noticed that Cadsoft Eagle can import DXF files too; I might see if it does any better with importing drill holes.
Most CAD flows import DXF as for outline handling, and they design for portable first, so expecting to extract PAD stack and Drill information, is
maybe expecting too much.
If you want full information flow, you should be able to define PAD sizes on all layers, as well as Paste and Mask separately, and drill with plated/non plated choices.
I've not seen a generic DXF import go to that level, but I have requested that KiCad add a tool/macro to the Footprint editor, that can extract a circle or polyline, and generate a PAD definition or hole definition. - ie the simple footprint helper stuff.
The user would still need to select item, then select what to create, using that as seed.
Possibly, some layer names could be used to assist seed process, but with things like offset drilled oval pads, getting more automation would need more code - enough to scan for 'Drill-contained-within'
It is still
technically possible to include PAD stack and Drill info in a DXF file, and Mentor for example, have two DXF export choices:
Flat DXF, which is close to a plotter, with no database structure - but it is highly portable.
Full DXF uses DXF comment fields etc, to tag entities so they can import back as PAD stack, Drill info outlines and rules etc.
This one is less portable, and often leads to complaints of clutter, for tools that ignore hidden attributes.
If you had control of the sources of both the EDA tool, and the DXF generator, you could, in theory, get a similar result.