> I'm a big fan of "drawing" my footprints with either a text editor or > a python script. It's been a while since I last did this, and I know > that pcb keeps changing. Is the documentation at > http://pcb.sourceforge.net/pcb-20070208/pcb.html correct for the > 20070208 snapshot? (Or is there any compelling reason to us the CVS > version?)
CVS has arbitrary element rotations. I don't think we've changed the format since then. > Second question: if I want to draw a dot on the silk layer (i.e., a > filled-in circle), am I to use the ElementArc command with x,y at the > center, thickness equal to the desired radius, a width and height > equal to half the radius, and a delta angle of 360? (Or is that angle > in radians?) ElementLine from X,Y to X,Y, thickness = diameter. The code knows to draw that as a filled circle, since we use that to draw BGA pads. Using ElementArc would draw a circle, not a dot. In theory, you could get away with it if you chose radius and thickness equal to *half* the dot's diameter, though. > And lastly, what is the "best practice" on placing the mark and > element text? Seems to me that the mark should either be in the > center of the element body or centered on pin/pad 1. I've always > just left the text at the origin and moved/rotated it during layout. I put the mark at the center of the part, if that makes sense to. For odd-shaped parts, I put it on pin1. Either way, I keep the mark and the pins on the same grid. I put text inside the element if I can, but I always end up moving it during layout. The latest PCB has a "lock text" option that keeps you from accidentally selecting the names when moving elements, and an "only text" mode for rearranging the refdes's. _______________________________________________ geda-user mailing list [email protected] http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
