Cutter Comp in control

[kennebec]

I am using a 1/2 Ø x 90° spot drill to deburr parts, I run comp in control and set comp at tool Radius .02 deep (D=.02) I program Z-.03 this gives me a .010 chamfer. My problem is going into small corners in this case a .094 rad corner the arc is converted to 2 xy lines rather than R.094, (Mcam looks at the tool I have chosen, a 1/2 Ø and adjusts the program for it, well if I run the program with .02 comp the tool travels by my .094 R until the 2 larger entities I have filleted with the .094Radius intersect, any easy fixes? I wish the with comp in control Mcam would look at the entities with a zero tool dia, just drive the Geometry. We do not program offline that has been tried and suggested.

[Josh T™]

Can you post a file on the FTP site?

[cunder]

I would change the tool type to a chamfer mill and use the contour type as 2D chamfer and see how that works.

[Midwest]

Try using "Wear" for your cutter comp

 

 

HTH

 

 

[Grievous]

Uncheck " Optimize cutter comp in control" button

[PeterM]

You are programming chamfers more or less the way I used to back before V9.

First, find out the effective flat of the spot drill that you are using. Modify a chamfer mill in the Mastercam tool library to show the same flat that the spot drill has, this way Mastercam can calculate the chamfer accurately, and verify will show an accurate chamfer as well. Then use the chamfer mill tool type ala cunder, but keep the tip offset small enough that the smallest corner radius of your geometry is that small, or larger, if you cannot make it that small, the simplest solution is to copy the contour geometry to another level, and trim those corners sharp. I personally don't use any ccomp for my 90 deg tools, it's just as easy to adjust the z offset, but that's a matter of preference. If you insist on using comp in control, remember that the inside corners either need to be sharp, or larger than the effective radius of the tool, or you will get alarms at the machine.