Manufacturing Information Solutions

[dawn]

I use FeatureCam 2.5 at work to prg a centroid controlled machine. My question has to with part line progamming. I usually just leave the part line prg box checked in my program and tell it what size tool I am going to be using, when I do this I have no control at the machine to adjust for tool wear. Usually this is ok because I do mostly one off parts. The other day though I was doing multiple aluminum cover plates. The plates had 8 .530 bolt holes and a .250 wide groove for a o-ring im guessing. Anyways i set the program to pre drill the holes to .500 and then circular interpolate them to .550 i had partline prg checked and cutter comp checked so that i could adjust for wear out on the floor. For the slot I set it to use a .1875 emill with cutter comp checked and partline checked. The slot worked fine it came out right to size. The hole on the other hand got chewed up. It programmed the tool to cut on the outer tool path instead of the inner tool path. So aft some head scratching I unchecked part line prg and left cutter comp on for the hole and it worked fine. Im just stumped, why would it work on the slot and not the hole. If any of you guys know what I am talking about or could give me a better explanation as to when I should use part line and cutter comp or shouldnt as in this case I would greatly appreciate it. P.S. I hope all you guys are getting busy are shop has been swamped with ork for the last few months and it sure is nicer than trying to look busy.

[mistux]

You probably have overlooked the DIRECTION of cut.

G41: cuts on the LEFT side as the cutter moves AWAY from you.
G42: cuts on the RIGHT side as cutter moves away from you.

Do you have some sort of backplot or display capability so that you can see what the cut will look like?

[JamieR]

First of all, I never program anything without including cutter comp. Even on one-off parts. What amount of diameter offset did you have in the machine control for the tool that did the .530 holes? In "part line prg" you are programming with the center-line of the tool on the part geometry and letting cutter comp at the machine offset the tool paths by the amount of offset you have entered into the tool data. If you are NOT using "part line prg", then the cam software will offset your toolpath to the left or right of the part geometry. So, when using "part line prg" you enter the actual diameter of the cutter as your offset at the machine control. When NOT using "part line prg" you enter the difference between the actual cutter diameter and the diameter the CAM software used to offset the tool paths.
Cut direction is another factor, as mentioned above. I'm not real familiar with FeatureCam but I'm sure it has some type of verify or backplot feature so you can see which side of the geometry the cutter is on. If it is on the wrong side, you can either reverse your cut direction or switch between cutter comp left/right.

In your situation, since the program worked fine when you unchecked "part line prg", I'm guessing that either the cutter comp left/right needed switched, the wrong amount was entered into the tool offset data or both.