Steve Wiseman wrote:
> 
> If I could run the
> error-checker over the gerbers, to check for continuity, that'd be great,
> but that's not (yet) an option.

This is what I do on simple boards (without power planes) to check the
positive gerbers with my original DRC settings:

1. Delete all polygons, tracks and arcs.

   (Create a selection query (Edit, Query Manager...) with a name like
   "gerber check" and with these statements:
   select all polygon.grid which are greater than or equal 0 and
   select all track.width which are greater than or equal 0 and
   select all arc.width which are greater than or equal 0.0

   To be on the safe side check De-select All before applying the selection.
   Complete this step with Edit, Clear or Ctrl+Del.)

2. Globally change all pad X,Y sizes to 0 (zero).

3. Globally change all via diameters to 0 (zero).

4. Import your gerber signal layers.

5. Choose Update Free Primitives From Component Pads in Design,
   Netlist Manager, Menu.

6. Run your original DRC on the board.
   (If I use the 2:3 format, which has a 1 mil resolution, I usually have
   to reduce my original clearance constraint by 1 mil to get rid of a
   few violations caused by the gerbers.)

Sadly enough, missing pads will go unnoticed if you follow the good
practice of always routing to or from the centre of pads. But otherwise
the described method has worked for me and only takes a few minutes to
set up. It may contain some redundancy or lack important points so any
comments are welcome. 

Gyula Hegyesi

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
*
* To leave this list visit:
* http://www.techservinc.com/protelusers/leave.html
*
* Contact the list manager:
* mailto:[EMAIL PROTECTED]
*
* Forum Guidelines Rules:
* http://www.techservinc.com/protelusers/forumrules.html
*
* Browse or Search previous postings:
* http://www.mail-archive.com/proteledaforum@techservinc.com
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Reply via email to