Are you taking a skim cut over the top of engraving, to deburr?

Hi guys,

I've been having to take a skim cut after engraving in 6061 and 7075, to deburr. I'm using Harvey 963230-C8 2-flute .01" web TiB2 coated engraving cutter. This tool is supposed to be the s__t for engraving aluminum, at last according to Harvey . The engraving itself is lovely, but it invariably raises burrs that I need to knock down.

16,000 RPM
.0015" chipload (48 IPM)
.01" - .015" depth
Good coolant and machine, everything else looks fabulous

I could slow down maybe, but that would end up taking longer than just taking the skim cut.

Is this typical? Am I just dumb?

Thanks, and regards.

Mike

I just engraved 2024 today, 12k rpms 10 ipm .006 doc...no burrs using a #1 centerdrill. I prefer to do steps of .005 for deeper engraving no matter the tool.

I usually run at 20 ipm but for some reason I put 10...oh well it was only like 100 numbers and letters...

I think those Harvey engravers suck,TBH. I find a good #1 centerdrll or ball mill works best in 6061. I am currently using a .05 diameter ball mill .004 deep 30 ipm and 4k. .25" text gets weird if I feed faster.

Forgot to add I NEVER TAKE A SKIM CUT TO DEBURR.

we do all our engraving with a ball em, no deburring necessary.

I agree with using a ball vs. "engraving" tool. A good ball mill will have less than a .010" web. And more positive cutting edge.
Unless you need a super fine line. Then I have had better luck with single fluters.

Only issue with a skim cut is you may roll a burrito (yes it autocorrected to that, I left it for the lulz) into letters. I have found that square endmills tend to raise a burr way easier than a ball, centerdrill, or even a custom ground 3 sided tool.

If I have to have flat bottom letters I'll wait to do my surface finishing then hit it with Emory and scotchbrite. That takes care of the burrs and knocks out the finishing in one step.

IMO, that is feeding about 5x as fast as I would.

PM

12k, 35 IPM feed, 8 IPM plunge, .003-.004" deep, 1/32" 3 flute ball nose. .005" feed height, .010" rapid height. 12 years in the Haas and never seen one burr.

Burrs have been a problem for me using centerdrills, ballnose, engraving bits, just about anything. I hit them with a abrasive brush mounted in the changer.
Given feed rates mentioned at what point does a 8 to $10,000 laser make more sense for engraving at a dollar or two per minute?
Bob
(yes, I know I'm being bad and straying off the original question, just curious as to viewpoints)

I agree Ballmill. But I think maybe way too deep, .015" so you're getting a .0259" wide path, with a 60º Tool. If that's the width you need, I would use a larger diameter Tool and less depth. Obviously not to the extreme where it shows up smeary. That's generally why people use Ballmills.

R

Here are a couple examples:






1/4" tall letters, ~.025" line width. Sanding the burrs down would kill the aesthetics.

Engraving these letters takes ~20 seconds, and the skim cut takes ~5 seconds including the tool change.

Maybe 48 IPM is way too fast, but I've done ~500 parts so far with the same cutter so it's not killing the cutter.

Regards.

Mike

I used to engrave a lot of aluminum at a past job, though not on a production basis. These were "showcase" pieces that had to be perfect, so trying to touch them up after machining was not an option with emory or scotch brite.

A few thoughts, mostly to echo previous posts. If your engraving needs to be .01-.015 deep, I would machine nearly to depth, leaving a cleanup pass, I would do something like .009/.001 or .013/.002 or similar. Your depth has a lot to do with the burr, at that depth, and your speeds and feeds, and especially 6061, your pushing a lot of the material. I also found with this process, running the first cut like hell and then a moderate clean up pass worked well. Course running both at moderate feeds worked well too.

In regards to the cutter, I, personally, have found Harvey tool is like a drunk guy at a bar bragging about... pick a subject. Their claims far exceed their abilities. Personally I use a chamfer mill for most of my engraving. If I had the cash, or a production job that paid for it, I would buy a Helical Chamfer tool like what Scientific Cutting Tools sells.

Last thought, trying to guess scale from the leather grain and the loops on the towel, those letters are fairly large. I use an 1/8" cutter for TINY lettering, typically .003-.005 depth. I would use a larger cutter, as large as you can clear with the numbers being by the wall of the part. Even stepping up from an 1/8" to a 3/16" will help, especially with the depth you are cutting.

I do all my chamfering and engraving with "chamfer mills" or whatever you want to call them. The little guys I buy cheap Melin or similar, the bigger guys I have my tool grinder regrind into chamfer mills when they don't have enough flute length left to retip. Another benefit when you step up in size, you can be using 4fl instead of 2.

I use Onsrud engraving cutters............Eh............they work great until they wear a little. The problem comes from the cutting speed at the tip of a .005-.010 Ø cutter...............should runnin around 500k+ rpms or so in Ali.............

Finegrain said:

Here are a couple examples:

1/4" tall letters, ~.025" line width. Sanding the burrs down would kill the aesthetics.

Click to expand...

Let's talk aesthetics as it does count very big in marking.
What is with all these "dots", the 4's look, ... well not just very clean.
Why?
A guess is the corner stop needed, would a font with a small rad engrave better? Are there such fonts for cnc engraving that are machine friendly out there?
I do hate seeing start and stop points in engraving. It just makes it look not right. You would never allow this blip on a die or mold.

I'm not "sanding" the top, more polishing it using fine grits (800 grit de-burr flex abrasive is common in my world) but that is not gonna work in a recess like you have here.
Bob

I am engraving some real fine lines in 6061 now (.005" tip, .004" deep). I tried the 2 flute harvey tool cutters and was not at all impressed. I switched to a single flute traditional engraving cutter from 2linc and it is much nicer. No discernible burrs. Looking at the engraving from the harvey tool cutter under a microscope did not look like it was really cutting, or at least not well, but just plowing through.

Pete Deal said:

I am engraving some real fine lines in 6061 now (.005" tip, .004" deep). I tried the 2 flute harvey tool cutters and was not at all impressed. I switched to a single flute traditional engraving cutter from 2linc and it is much nicer. No discernible burrs. Looking at the engraving from the harvey tool cutter under a microscope did not look like it was really cutting, or at least not well, but just plowing through.

Click to expand...

Well, depending on diamter, it probably wasn't cutting... Knowing this from running .007" and larger endmills with only 10k rpm... Use a ballmill for engraving like everyone else said...

CarbideBob said:

Let's talk aesthetics as it does count very big in marking.
What is with all these "dots", the 4's look, ... well not just very clean.

Click to expand...

Well that's the trick, right? Cutter needs to have a rather sharp tip so that it can pull up out of the corners and leave them as square as possible (look at the "7" in the 2nd photo), but also then a sharp cutter needs to run deeper to get a uniform floor. Neither a BEM or a regular with larger tip would be able to square out the corners.

Regards.

Mike

Basset makes a super strong .021 ball endmill for engraving purposes. Use them on every machine but I'm engraving .005 deep max. No burr or necessary clean up afterwards

I'm gonna engrave the exact same numbers tomorrow and see how it looks in 2024...what's the font?

Mike1974 said:

Well, depending on diamter, it probably wasn't cutting... Knowing this from running .007" and larger endmills with only 10k rpm... Use a ballmill for engraving like everyone else said...

Click to expand...

I have no intention of using a ball endmill. What is being described with everyone using a ball endmill is a cutting a shallow semicircular ditch- not what I am after. I want a cut with more vertical side walls. What I am doing is working so far. When I have a problem we'll see.