How do I use the Eagle ARC command

Community PCB Design
1

I have spent the day trying to understand how to use the ARC command in Eagle.

I want to draw a 90 degree arc with it’s center at 0.5, 1.7 and its radius 0.5 (units are inches here).

I want it to start at 270 degrees and end at 360 degrees. HOW!

Any enlightenment will be appreciated.

Vic

2

I sorta liked the EAGLE manual explanation; it made sense when

compared to the way the GUI arc command worked:

The ARC command, followed by three mouse clicks on a drawing, draws

an arc of defined width. The first point defines a point on a

circle, the second its diameter. Entering the second coordinate

reduces the circle to a semi-circle, while the right button alters

the direction from first to second point. Entry of a third

coordinate truncates the semi-circle to an arc extending to a point

defined by the intersection of the circumference and a line between

the third point and the arc center.

So if you have a center (X,Y) and a radius R and a thickness T, you

need a command like:

change width t; arc (x-r y) (x+r y)

(and then click to make the other endpoint)

Polar coordinates may also be useful; they’re relative to mark, and

generally a lot more convenient when you’re dealing with curves…

change width t;mark (x y); arc ccw (P R startAngle) (P -R

startAngle) (P R endAngle)

You might also look into the “wire” command, since in recent versions,

ARC are just a special instance of curved wires.

For your particular example, try:

mark (0.5 1.7); arc cw (p 0.5 0) (p -0.5 0) (p 0.5 270);