Deflection Kills an Endmill

Dec 16, 2011 // by page.lysupportadmin // Blog, Software, Techniques // 2 Comments

I enjoy watching John Grimsmo’s knifemaking videos, so I was recently catching up to see what I’d missed. I will show a couple of the good ones in a second post, but first I wanted to touch on a case where deflection broke an endmill. John’s video captured it perfectly at about 9:22:

Tool deflection breaks an endmill

You can tell by the waves on what should have been smoothly flowing walls in the slot that this endmill was deflecting quite a lot. Too much as it turns out, because it broke…

He’s pointing at the path where he was profiling the edge of a knife blade with a full slot cut, 1/8″ endmill, 1/8″ deep. I don’t have all the data to tell how to set this cut up in G-Wizard to see recommended feeds and speeds, but you can see by the waves in the slot that the tool was deflecting quite a lot. If I just run some sample parameters for a carbide endmill, and assume a stickout of 1/2″ for the tool, I get a recommended rpm of 4600. If I then plug in the 4.5 IPM he said he was running, I notice a couple of things.

First, predicted deflection is 0.0009″, whereas 0.001″ is really the limit of too much deflection. A little more rpm or a little more stickout, and we’d be well into the 0.001″ danger zone before we knew it. A stickout of 0.6″ yields 0.0015″ deflection, which would likely break the endmill right away.

Second issue is the chipload. John feels he is being conservative by feeding very slowly. However, he’s cutting 304 stainless, which is a work hardening material. The chipload in my test case with 4600 rpm at 4.5 IPM is only 0.0002″. These very light chiploads can easily work harden the material and make it much harder to cut than expected, and once again we may break the cutter pretty easily.

How to avoid these issues?

First, choke up on the tool as much as possible to minimize stickout, especially with these small cutters. Going from 0.5″ stickout to 0.4″ stickout would’ve reduced deflection from 0.0009″ to 0.0005″, which is almost half as much.

Second, beware feeding too slowly in work hardening materials. In, beware for nearly any material. It’s worse in work hardening materials, but even in non-work hardening you will eventually make such a light cut that your cutter “rubs” instead of cleanly shearing the material. See this page from our Feeds and Speeds Cookbook for more on avoiding the rubbing.

Sometimes machinists feel like they’re babying the tooling with slow feeds, but as you can see, it often is much harder on the tool.

For John’s knife project, some time spent with G-Wizard trying to keep the chipload where it was recommended, minimizing stickout, and possibly dialing back G-Wizard’s “Tortoise and Hare” slider to the less aggressive “Tortoise” side would help.

If you want to see the mishap from start to finish, go to about 8:00 in the video. He loses an endmill plunging too. Personally, I hate to plunge unless I just have to. It’s the hardest way to introduce a cutter into the material. A ramp is better, a helix is even better because it gets away from slotting while the ramp slots the whole way, and predrilling a hole is even better. In this case, one of the toolpaths where the ramp follows the profile would’ve been gentler on this tool. John uses SolidCAM, but I’m not sure whether it has that kind of entry option.

Okay, read on to the next few posts to see some cool stuff from John! BTW, the video I linked to is part of his “Knifemaking Tuesdays” series. He’s attempting to do a complete custom folding knife in CNC on a hobby class mill and making great progress. I love the idea of being able to CNC profile a blade rather than having to learn the art of hollow grinding on a belt sander.