Lately I’ve had several questions about how to set up GW Calculator for Chamfering. There’s two ways to go–you could set things up as a 90 degree V-Bit or you could set it up as a tapered endmill. Unless you’re using a V-Bit (i.e. a cutter with no real flutes), I recommend the latter. You used to have to do it V-Bit style before we introduced the Tool Geometry button and the possibility of tapered endmills.
There is one tricky aspect to it, and that is the difference in geometry between a chamfering tool and an endmill that’s tapered. Tapered Endmills typically have a gradual taper that’s used to put draft on the walls of a mold cavity and chamfering tools are all about the end having a fairly abrupt taper (typically 90 degrees). Here are some typical chamfering tools from Harvey Tool for example:
All the cutting is to be done on the angled nose and not on the sides. G-Wizard assumes the taper extends the full length of the stickout, so if you’re trying to specify a tapered endmill, you’ll need to make the stickout the flute length. If you have a chamfer tool, the stickout is the length of that angled area. For a 90 degree 1/2″ 4 flute chamfer tool, use 1/4″ for the stickout.
Let’s make that concrete. Here’s the geometry (accessed by selecting an endmill and then pressing the “Geometry” button) for a 1/2″ 90 degree chamfer tool:
As you can see, I have set the stickout to be 1/2 the cut diameter because it is a 90 degree chamfer tool. That also means the Taper Angle is 45 degrees, since we measure only half the total included angle to get the taper of a cutting flute. Okay, now let’s take that geometry and see a typical Chamfering Feeds and Speeds example in 6061 aluminum:
Some things to note:
– I have turned the “Tortoise/Hare” slider at the bottom to “Full Tortoise” to improve surface finish. Chamfering isn’t a roughing operation, so we want less feed relative to the spindle rpm to improve the finish.
– You can see the effective diameter for this cutting depth is 0.182 down in the HSM are right below the “Est. TEA” button.
This yields a recommendation of 5100 rpm (as fast as the Tormach spindle will go, and the orange is indicating GW would love to go faster if it could) at a feedrate of 59 IPM. Can we go slower to improve the surface finish further? Sure, there is no rubbing warning. By manually overriding the feedrate, I can see that the rubbing warning hits at about 17 IPM, so we can go quite a bit more slowly. Before just dialing things down to the minimum feedrate, you should try some experiments and see how much slow down really shows noticeable finish improvement. I’d do that with a few experiments until I quite seeing a difference. Machine a stepped surface and try successively lower feedrates from 59 down to 17. Once you can see where going more slowly quits being worthwhile, you’ll have learned something valuable. Note that information down, and in particular, note the chip load, because that’s the part that’s reusable for a variety of different circumstances, provided we’re talking about the same material. You might also want to note down faster feedrates that are “good enough”. You might also try something less than “Full Tortoise”. Depending on your machine, you may be able to go quite a bit faster while still getting acceptible surface finish.
If you haven’t tried the G-Wizard Feeds and Speeds Calculator and would like to learn more, check it out by clicking the link.
Software that will make anyone a better CNC'er
Get Better Tool Life, Surface Finish, and Material Removal Rates Fast.
It's that easy. You can install and get results in a matter of minutes.
Like what you read on CNCCookbook?
Join 100,000+ CNC'ers! Get our latest blog posts delivered straight to your email inbox once a week for free. Plus, we’ll give you access to some great CNC reference materials including:
- Our Big List of over 200 CNC Tips and Techniques
- Our Free GCode Programming Basics Course
- And more!
Just enter your name and email address below:
100% Privacy: We will never Spam you!