--- In [email protected], "yajeed2000" <[EMAIL PROTECTED]> wrote: > > Hi, > How is the offset adjust for drill and place files used? > At the moment when plotting my pcb the drill holes do not line up with > the pads in the gerber output. What is the procedure for using the > offset tool in Kicad to line them up properly? > Any help would be appreciated, Thanks. > > David. >
Offset adjust is for setting your own XY origin on the PCB layout. To use it click the "Plot Origine" radio buttons in both Plot and Drill menus when generating Gerber and drill files. 1) "absolute" is the default origin in the upper left corner of the PCB with both X & Y positive as you move towards the lower right corner of the PCB. 2) "auxiliary axis" is an origin of your choosing using the "Offset adjust " button (right hand side menu, bottom button). In addition there is a Mirror Y Axis check box in the Drill menu that can give unexpected drill file results if your not aware of it. My personal preference is to set a XY origin on my PCB (preferably a tooling hole), click the "auxiliary axis" buttons in Plot & Drill and uncheck the "mirror y axis" and "minimal header" boxes in Drill. That way the origin is set to a known point on the PCB, which makes dimensioning of the PCB Fabrication drawing easier, especially if the PCB has a unique shape. In addition the drill file now has an easy to locate reference point in common with the Gerber files. Regards, Dave G.
