[colton_m]

Hey guys,

I'm having a bit of an issue defining a chamfermill correctly.

The tool I've got is a 9Nine chamfermill, it's a single insert 90 deg chamfermill. The insert has a .8mm nose radius.

My question is how do I define a chamfermill with a nose radius and one flute?

I've selected chamfermill and set the following,
Outside Dia: 0.586"
Taper Angle: 45
Corner Radius: 0.031496 (0.8mm)
Diameter: ???

It makes sense that the "Diameter" should be zero because this tool doesn't have a flat on the tip, but no matter what I try the preview of the tool looks like some kind of wonky dove-tail cutter.

Any ideas?

[Superman]

To describe it correctly
- assume a flat plane at the tip, the 45° edge intersects the flat plane
- from the centreline to the intersection point is a radial distance, double it-------this is the base diameter that is placed into the tool description

NOTE---to get correct chamfers, the tool must contour any profile with the nose radius below the lower edge of the chamfer

[colton_m]

To describe it correctly
- assume a flat plane at the tip, the 45° edge intersects the flat plane
- from the centreline to the intersection point is a radial distance, double it-------this is the base diameter that is placed into the tool description

NOTE---to get correct chamfers, the tool must contour any profile with the nose radius below the lower edge of the chamfer

It doesn't seem to be working for me, I've tried 0.0445" and 0.0261" for the diameter, it still looks wrong. Here are some pics:

http://i19.photobucket.com/albums/b1...psa93daf62.jpg

http://i19.photobucket.com/albums/b1...psea55cecc.jpg

[Superman]

Ah, no,....I didn't mention nose rad values.... only that it must be below the lower edge

Corner radius IS...... zero
base dia IS..... 0.0216" (theoretical)

try this way
- create a hole....say 1.0000"
- set chamfer tool base dia to 0.080"
- in Mastercam, create 2D Chamfer Toolpath, geometry=select 1" circle @ 0 plane...... chamfer size= 0.010", tool project past by 0.060", wear comp.... ...top of stock=0 ...depth=0
- in control, set diameter comp to zero, run toolpath, adjust the tool base diameter ( smaller ) & repost, until the diameter of chamfer is 1.0200" (.....should start cutting at around Ø0.050")

the 9nine tool needs to be set larger, as the tip is slightly off centreline ( so the other side( of the 90°) will not drag on the part while it is cutting)
you will find limited success with spotting, and find that doing the larger chamfers is OK...but slow
- I tend to use a 1/4" carbide NC spotting drill for spotting & doing smaller chamfers,,,,2 cutting edges......goes 2X faster....., cuts cleaner