Stats

  • Locked Locked
  • Replies 3
  • Subscribers 166
  • Views 13943
  • Members are here 0
More Content
This discussion has been locked.
You can no longer post new replies to this discussion. If you have a question you can start a new discussion

My PCB Manufactuer claims my drill file is empty

James4235

Hello, I've followed the tutorial here to generate my drill file http://referencedesigner.com/tutorials/allegro/allegro_page_9.php and I have even viewed the drill file on an online gerber viewer and I can see the holes, however, my manufacturer (ALLPCB) says the drill file is empty. I have attached my drill file to this link https://ufile.io/r9pb4, can anyone spot anything wrong with it? Many thanks.

Parents
  • excellon1

    Hi James, I can confirm your drill file is not empty but what's going on is more than likely their tools are choking on what Allegro is putting out.

    Try this.

    NC Parameters:
    Enhanced Excellon Checked "Believe you have this checked"
    Trailing zero suppression checked.
    Coordinates = Absolute
    Output Units = English
    Format = 4 4 "Your format may be different"
    Offset x, y = 0

    NC Drill 
    Auto Tool Select Checked "Your file looks like it has not got this enabled"
    Repeat codes Checked
    Optimize drill head travel.

    After you generate the NC file, check the log. (View Log Button)

    I did some tests with a high-end, industry standard gerber editor that is capable of pulling in NC drill files. When using Enhanced Excellon format and if "Auto tool Select" is not enabled The gerber editor will not import the allegro NC file. "Probably an Allegro Bug"

    Give the above a try and see if all is working.

    Paul.

  • James4235
    in reply to excellon1

    Hi Paul, I followed your steps and the PCB manufacturer has now approved the PCB for fabrication, thank you for your help!

Reply
  • James4235
    in reply to excellon1

    Hi Paul, I followed your steps and the PCB manufacturer has now approved the PCB for fabrication, thank you for your help!

Children
  • excellon1
    in reply to James4235

    Sounds good James.

    Glad that worked out

    Paul

Cadence Guidelines

Community Guidelines

The Cadence Design Communities support Cadence users and technologists interacting to exchange ideas, news, technical information, and best practices to solve problems and get the most from Cadence technology. The community is open to everyone, and to provide the most value, we require participants to follow our Community Guidelines that facilitate a quality exchange of ideas and information. By accessing, contributing, using or downloading any materials from the site, you agree to be bound by the full Community Guidelines.