[MauserBob]

Hello all.

First, a little background.

I'm programming for a pair of Hardinge VMC-1000's running OM series Fanuc controls. The work I do involves machining flat panels of polycarbonate and acrylic into smallish parts that vary in size but usually average somewhere under 12" square. The parts I make are normally no thicker than .200" and almost always have a mylar conductive film of .007" thick laminated to either one or both faces of the material. Machining the mylar often results in a burr on the edges of the parts, so we use a dovetail tool to deburr the top and bottom edges. This works great on square-cornered parts as it produces a nice & even light chamfer all around the four sides. Occasionally, however, our parts require radiused corners....when this is the case, we usually get an heavier chamfer around the radius. It's usually acceptable, but in order to keep it in tolerance we will program a slower feedrate on the radius moves, say, F60 around the radii whereas we can run @ F180 on the straights. It works, but it's kind of a drag to have to slow down on the corners, especially on multiple part layouts.

So.....sorry for the long read, but I thought I had to set the scene. Anyway, while flipping through the Fanuc OM manual in search of an answer to another question, I discovered G39. The manual isn't entirely clear on it's purpose, so I don't know if it'll do what I want, but it appears to alter a toolpath around sharp corners on irregular shapes so as to more accurately produce the required profile. Now, it didn't really explain whether G39 is useful on 90 degree corners, nor did it show whether it would work around radii, but I'm intrigued nonetheless.

Anyone have any thoughts that might help me understand this G-code?

Any tips as to how I would program this code to run around, say, a 4" square part with .060 radii? Please feel free to offer suggestions.

Thanks in advance.



Rob.

[Andre' B]

The G39 command is not for putting a radius on a corner, it will if you lie and set the radius comp to something more then what the tool really is.

On outside corners G39 makes things smoother looping the tool around a sharp corner at the radius of the tool. Without it on a 90° the tool will go one radius past the corner make a sharp (high acceleration) change of direction.

On inside corners it can have a real effect (bad) on what the part looks like.
With it turned off you get what you normally want the cutter switches to the next move as soon as it is tangent. With G39 on the cutter will continue to the end of the current move make an arc back around the intersection point and start off in the new direction, this puts two gouges in the corner.


Edit:
What you are looking for is called corner rounding, and if your control will do it should look somthing like this.

(A 4" SQUARE WITH A 1/2 TOOL AND NO RADIUS COMP)
G0 X-1.0 Y-1.0
G1 X-0.25
G1 Y[4.0+0.25],R[0.25+0.0625]
G1 X[4.0+0.25],R[0.25+0.0625]
G1 Y[0.0-0.25],R[0.25+0.0625]
G1 X[0.0-0.25],R[0.25+0.0625]
G1 Y[0.01+0.0625]
G1 X-1.0

[MauserBob]

Okay. Thanks, Andre.


Rob.