On 07/03/2012 11:42 AM, jean-pierre charras wrote: > Le 03/07/2012 17:16, Dick Hollenbeck a écrit : >> On 07/03/2012 05:09 AM, Carl Rash wrote: >>> Dick, >>> The diameter of the hole and the diameter of the via pad are correct >>> (verified with 3rd party gerber viewer), 0.015 and 0.025. The problem is the >>> hole is off center. I believe this code in gendrill.cpp is selecting the >>> size of the drill and that is correct. It may be that placing a hole within >>> one half a mil is not possible using the NC format if that is the case then >>> I would have like to have it detected at the DRC phase and not after >>> submission to the PCB fabrication house. Perhaps a minimum annular ring test >>> would be a good DRC check. >>> I am going to try and change the next grid hot key to a combination like >>> Ctrl+G that way It will not be likely that I can inadvertently change grid >>> size without knowing it. I have never used auto routers, I prefer to do it >>> myself so I depend on the grid staying where I set it. >>> >>> Thanks for time >>> Carl Rash >> Is there actually a bug here? >> >> It is sounding like a user error, not a true bug. >> >> It is fully understandable that you do not like the current functionality, >> which might be >> validly classified as something other than a bug. > > In fact, this is a truncating issue in Excellon drill file, not an actual bug > in pcbnew. > The coordinates were truncated to 3 digits after the decimal point, > giving a 1/1000 mm resolution when the file is in mm (this is the max > resolution allowed in Excellon files), > but only a 1/1000 inch resolution when the file is in inches (The max > resolution allowed in Excellon files is 1/10000 inch) > > This is not related to nanometer version, and, I am thinking, was a very old > behavior. > This truncation can be seen only for some grids like 2.5 mils, but there is > no bug inside Pcbnew. > > I fixed it, and just committed the fix > (For Excellon files in inches, the max number of digits is now 4, that is the > full allowed resolution).
The community owes you another thank you, Jean-Pierre. I wish it would happen. _______________________________________________ Mailing list: https://launchpad.net/~kicad-developers Post to : [email protected] Unsubscribe : https://launchpad.net/~kicad-developers More help : https://help.launchpad.net/ListHelp
