Using Tormach bit 34681 .125 engraving bit to make keychains with my students. After dulling the end of one of the bits already I am wondering what everyone is running for depth of cut and feeds and speeds for this bit.
Unlikely you “dulled” the end. More likely the tip broke off. Let us know: Which machine? What material? Coolant? This type of engraving cutter is probably best suited to high rpm shallow DOC and soft material.
Correct, I did snap the end off of the bit. I am using a Tormach 1100. We are machining aluminum with coolant.
give it all the rpms, maybe .0003-.0005" ipt feed .002-.005" DOC? I don’t run that style engraver anymore so I can’t offer a proven recipe.
Those engraver bits break very easily. I changed to chamfer mills after breaking 3 engravers on one part. Chamfer mills are about the same price more flutes and a lot tougher.
I’ve done a lot of engraving with the PCNC1100. I use the “half conical” type carbide engravers. (I don’t know the proper name for this type of engraver.) It’s been my experience that the tips will chip, but not really dull. It has also been my experience that the original geometry of the engraver will often leave burrs in the engraving. I’m running the spindle at top speed (5100 rpm) and I’m feeding at 5-8 ipm, which is fairly gentle. When engraving, the max Z depth is usually .004 - .008 in. I normally engrave with multiple passes.
What I mean by burr is this. When engraving, I use either flood coolant or I manually spray coolant from a spray bottle. When the part is done, I’ll wash coolant off with water and dry the part with a paper towel. The burrs in the engraving tear off little pieces of paper towel and make the part look bad. You can also feel the burrs with your hand.
So when the engravers become dull (or chipped tip), I load up a new one. Because they’re carbide, I could never bring myself to throw them away, and they accumulated. Same thing if I break or chip any carbide tool.
Then I got a Cuttermaster tool grinder and some tooling for it. I finally learned about the engraver tool geometry - specifically about how to grind a relief behind the cutting edge. Not only could I sharpen dull or chipped engravers, I could make additional engravers from broken carbide endmills. I did some experimentation with the geometry, and I can now make engravers that won’t leave a burr, whether I’m engraving aluminum, stainless, or even 6AL4V titanium. And yeah, after saving all those dull engravers and broken endmills, I now have about 30-35 engravers, some in 1/8", some in 3/16", and several in 1/4" diameter.
And yes, after the first couple of weekends with the Cuttermaster, every endmill, drill, countersink, and engraver I have is sharp.
-M
No I’m curious what kind of grind you are putting on that doesn’t raise a bur. That sounds like a fun rabbit hole to fall down. I am a big fan of running the superfly over an engraved part to take a thou of and clean everything up. Granted, that only works when engraving on the top surface of a part
Its hard to get enogh RPMs for engraving bits. Especially in soft stuff.