What's new
What's new

getting an angle when putting in an offset

skoobiz

Aluminum
Joined
Jan 8, 2007
Location
Hagerstown MD
Simple little question has anyone ever tried to take a shortcut by just using offsets when you don't have the tool a program calls for and it is a rush? Well one of my best guys did this on our HAAS VF 2 circa 1999. He needed a rounding tool to create a 1/4" radius. The program called for a rounding cutter with a 3/8" tip but all we had that was sharp was one with a 1/2" tip so he put in an offset to compensate for the difference in size. Much to his surprise when he ran the program he noticed that what was supposed to be a straight line cut was actually cutting a taper on the Y axis. It would start off cutting to much then slowly taper out to where it should be then it would cut fine until it got to the other end and again it would taper inward toward the part about .04". Is there a limit to how large of an offset you can add to a cutter in a HAAS? if so what is it? Has anyone else ever experienced this?
 
this is why it's important to understand how to correctly turn your comp on and off correctly. Post your code and I'll show you where it's wrong
 
Okay I will attach a copy of the program

in this section, you're starting at X10.65, you turn on your tool comp on the X7.6247 line. So the control is going to start at X10.65 Y-8.3325 with no comp. Now, on line 525 it's going to start comping and move to X7.6247 Y-8.3950. That's where your taper is. You just need to add a turn on line, Say on line 522 change to X10.75, then between line 524/525 add G1 G41 D4 X10.65 Y-8.3225. Make sure you do the same thing when you G40


N522 X10.65 Y-8.3225
N523 Z0.4325
N524 G1 Z0.02 F2.9
N525 G41 D04 X7.6247 F9.8
 
in this section, you're starting at X10.65, you turn on your tool comp on the X7.6247 line. So the control is going to start at X10.65 Y-8.3325 with no comp. Now, on line 525 it's going to start comping and move to X7.6247 Y-8.3950. That's where your taper is. You just need to add a turn on line, Say on line 522 change to X10.75, then between line 524/525 add G1 G41 D4 X10.65 Y-8.3225. Make sure you do the same thing when you G40


N522 X10.65 Y-8.3225
N523 Z0.4325
N524 G1 Z0.02 F2.9
N525 G41 D04 X7.6247 F9.8

Thanks Larry, I'll try that, it makes perfect sense. Actually I'm not sure why my CAM is posting it that way. I'll have to look a little deeper for that.
 








 
Back
Top