Is there a way to output a Gerber drill layer from Allegro

Not really..  Excellon is the company that makes the drilling machines that *all* the fabricators use that is why the format is supported.

In Gerber you can only get a "picture" of the drill symbols.  This could be used by someone but it's very labor intensive.

Why are you asking by the way?

In a previous life I was a CAM tech at a PCB fabricator.  Occasionally, I would receive  Gerber format drill layers instead of Excellon  format drill layers.  I usually preferred getting them this way as it saved a step during data input and eliminated any potential mismatch in data precession (# of decimal places).  

When I moved into the PCB design world I had been using ODB++ almost exclusively as that was the format the PCB shop I was working with preferred.   Last year, I moved to a new company and the PCB fabricators we use here prefer Gerber.  In lieu of getting the fabricator to accept ODB++, I thought if I could find a way to output Gerber drill layers I could save myself a step on output, save the fabricator a step on input, and potentially avoid data translation errors.

Excellon is pretty much the defacto standard for all drill data in PCB Design, that been said it would be possible to output drill data in gerber format or "Decode" size based on the actual drill size used. To do this one would need to create an additional layer in Allegro - Lets call it Drill2, in your padstacks you would need a padstack on that layer that is the same size as the drill. The padstack editor may not like this and tell you the pad will be drilled away but it is doable... When the gerber file is created for the desigm simply enable Drill2 and you will have a gerber representation of your drill hole sizes. What cam editor did you use to convert decodes to drill data ?, im curious about that. Thanks Scott

Thanks Scott, 

I was using Genesis2000. 

When an Excellon drill file is input into Genesis it become just another layer and can be manipulated just like any other Gerber layer. 

The process of identifying and translating  Excellon files into Genesis is slightly different than Gerber files which opens up possibilities for translation errors.  This is one of the benefits of using ODB++; the Drill data is already translated and ready for manipulation within Genesis.

I know Excellon is the "DeFacto" standard for sending drill/rout data between CAD (designers) and CAM (fabricators) - but it doesn't need to be.  Excellon is generally used by the fabricator to drive their drill/route machines.  As designers we are driving fabricator's CAM systems, not their manufacturing equipment.  Therefore we can (and probably should)  supply more robust data in order to make their lives easier. 

 

 

Yes, under artwork create FILMs that contains pin and via class for all of your drill layer pairs. Use the starting drill layerr for the class/subclass.  If you just have through hole technology you only need one additional film. On that film, check the "Draw holes only" checkbox (last entry on the right half of the artwork dialog).

When you produce Gerber using this film it will only contain the drills.

With this option you cannot include ETCH layers.