Brass feeds & speeds

[David Kenagy]

At last, I have the Onefinity working. My project now is a clock dial, etched in 1/32” brass. Parts of the lettering are very fine (only 0.008” wide at the surface). The parts that are wider (0.015”) need to be deep enough to accept the black wax that makes letters more visible. Having broken the tips off two blades, I’m asking whether to change settings, tools or goals.

The blades are single-flute inserts in the Amana (12 mm) shaft. They both are 30 degree V bits (solid carbide). The first bit had a tip diameter of 0.005”, and the second was 0.01”. Between efforts I got e-mail advice from Amana and after the second fail I spoke with them. Here are the set-ups:

Try #1
- Tip 0.005” (Amana RCK-360)
- 6000 RPM, 20 Inch/min (IPM per their table)
- Pass depth 0.008
- Full depth 0.015
- Left protective plastic on the brass

Try #2
- Tip 0.01” (Amana RCK-361)
- 6000 RPM, 47 Inch/min (IPM per their table)
- Pass depth reduced to 0.005
- Full depth increased to 0.02
- Took off plastic. (Flip side of the same sheet as the first try)

They suggested reducing both the pass depth and IPM by 50% (0.002” passes, and 20 IPM)

Though they were kind and are sending replacement blades, I’m not confident. Does anyone have advice on settings, or am I using the wrong tool for this job?

[Jim Becker]

Consider a diamond drag for the fine engraving.

[David Kenagy]

I was thinking similarly about diamond drag. Online, I see ads at $95-$120, but also a new offering from Carbide 3D. They want $40 for their "MC Etcher". Are the others 2-3 times as good, or likely to last 2-3x longer? What companies do you like for these cutters?

If I do the finest work with diamond drag, then I'll still need a V-groove for the (larger) Roman numerals. I wouldn't need a 0.005" tip, but my second effort chipped the tip off the 0.01" cutter.
I just ordered brass 260 (half-hard), and don't recall the specs on the sheet that just failed. I've read that brass 360 is "machineable" but it's not available from the source I've been using ("Online Metals"). Is there a 'best' alloy for this work?

[Jim Becker]

I don't own one, so I can't give you a specific reference. But check Amazon. Perhaps getting one on the lower price range to prove the method is worthy of consideration. I suspect the better tools will last longer as there are moving parts in diamond drags and the quality of the industrial diamond might also vary. But that's speculation on my part.

[Wes Grass]

'More Power' ... RPM, really. A .010 cutter is only 16 SFPM at 6k RPM. Run it as fast as you've got, probably won't go over 50 SFPM, which is slow for carbide even in a piece of steel. The other factor is feed rate. 20 IPM is ~.003/rev with a single flute. Not sure about that with brass. I hope the 47 IPM is a typo. May as well just drag it through the work with the spindle off ;-)

Another factor, probably one of the most important, is runout. It needs to be dead true, or at least off a *tiny* amount in the proper direction so the heel isn't dragging. Otherwise, you literally are dragging it thru the work. Roughly equivalent to running the spindle in reverse.

I haven't had much trouble with standard 'half round' engraving tools in my VMC, and it's only got a 10k spindle, which I rarely (never, really) run that fast. So probably 8500 for engraving. A program for aluminum I have on my PC here has 12 IPM at 8500.

****No idea what I ran in steel, but I tipped the tool off with a diamond hone first. These were 'sharp' out of the tube and break right off at contact.

Found ... pretty sure 416 Stainless: .010 deep, 9500 RPM, 4.75 IPM.

The other feed factor is depth. I try to ramp in if possible. These tools don't plunge well at all. Hard to do with lettering unless it's built into the control like my Fadal, or the CAM spits it out. Worst case, there's notepad ... and a lot of staring at the screen figuring out what's what.

Some of the numbers I've seen from cutter mfg'rs suggests they might be trying to sell more tools ;-)

[David Kenagy]

The specifics are helpful, Wes;

No typo, 47 IPM is literally what the Amana chart recommended for a 0.01 tip running at 6000 RPM. For 9000 RPM, the same cutter would run move at 71 IPM on their table. You meant the number is far from what you expected, but am I right that you meant much, much lower IPM? (I take that from your numbers after "416 Stainless"). Interestingly, the Amana table that says these are good for brass also has "Hard Wood" and "MDF" among the uses, but it's the same table for all.

So when those replacement blades arrive, I was going to halve the pass depth (0.002) and IPM (20). Putting your experience into the plan, what about increasing speed to 8000 (Spindle can go 24000) and reduce IPM to 5?

[richard newman]

I use a diamond drag tool on mother of pearl to scratch guidelines for hand engraving. I'm not sure it would go very deep at all in brass, the pearl fractures and turns to dust, while the brass would need to deform. I got my tool on ebay.

I've never engraved brass, but I have milled and turned a lot of it, and it likes high speeds. Wes is right about 47 IPM being way too fast, and also about runout being critical. There is a lot of good information on the PreciseBits site. Also look at the Roland and Gravotech websites, they make machines for engraving. You could also find an engravers forum and ask there.

[Wes Grass]

I looked at the chart. Umm, wow. For reference, 6000 rpm would be a reasonable speed with a HSS 1/8" cutter in aluminum or brass, ~200 SFM (100 mild steel, 50 tool steel). And I'd probably feed it 18 IPM (2 flute, .0015 per).

I'm kinda surprised by the price of the shank and insert. And I have to think there's likely an added runout situation by doing it that way. Maybe not an issue with wood or plastic, but ...

I'm assuming you have a 'spindle', with a direct ER collet interface? High quality collets help, and keeping the spindle bore and nut clean. I think there's an issue with dust from cutting wood and carbon getting up in the slots, and if it's not cleaned out at a bit change the collet irons it onto the spindle bore. I was able to literally feel it with my finger on the routers I ran at my last job. Lacking a tool to scrub it, a wad of medium steel wool twisted in there a bit, followed by wiping it out, helps a bunch. I think the bores of the router motors were far worse than the Avid spindle, just nowhere near the surface finish to begin with. Never mind the collet itself.

I'm using tools like this: https://www.amazon.com/LMT-Onsrud-Ca...001VXS1GK?th=1

Cheaper than the insert alone, and held directly almost guaranteed to have better runout. And if you can get away with a 60° bit, I've found them to be much tougher.

I got some recently from Lakeshore with a ball nose and spiral flutes. Haven't tried them yet, but I won't be surprised if they can't handle anything but aluminum. They sure look cool though.

Even on the CNC with carbide, I admit to being a wuss. With a 10k limit I don't have much option with small tools, but I baby the bigger stuff too. Almost always prototypes, so saving cutting tools and not screwing up is more important than cycle time. Even the 'fast' machine I'd like to get is 'only' 15k.

Way back in the 80's I went to a 'machinery show', an open house at a dealer. They were running a demo on a mill, 1/2" 2 flute cutter pocketing aluminum at 12k rpm and 240 IPM. They had an issue to work out getting the pocket started without 'ram-horning' the cutter while it was cutting full width. But once it got to profiling it was awesome to watch. I never thought anything that big and heavy could move that fast. That maker has been on my dream list ever since. Better get moving on it, I've probably only got 10-15 years left to wear it out ;-)

416 SS. Engraved soft and then hardened so the 'black' was left in the engraving when I polished the outside. That program also has 9500 RPM, and 4.75 IPM, and the tool notes say a 30° cutter. No doubt tipped off.

port_2.jpg

[Tony Leonard]

I use the cheapie bits from ebay that are 1/8" shank (same half cone shape). I have never broken one. I am using a router (Bosch 1617) set to probably 18000 RPM. I make 0.010" or so passes with no issues at around 50 ipm. I have used these bits and speeds for lots of brass, aluminum, slate, marble, etc. I think the cheapie bits are 30° with a 0.007" flat on the bottom? I've filled the engraved text with enamel paint before and it looks quite nice. That being subjective, I recall that you are looking for a whole different level than what I am. But I think you are on the right track anyway. How do you set your Z zero? Could you be plunging more than you think? Even still, I have made 0.020" passes with no problem before. I use these same bits for engraving circuit boards (copper and phenolic) - line width is critical.

I made a spreadsheet to calculate the width of the lines based on the depth of the 30° bit. That helps when trying to make real fine lines.

Another thing I ran into was flatness/thickness of the stock. If everything is not consistent, I get noticeably different widths.

Diamond drags are great for come things, but based on the one I have, I get better results with the engraving bits for this sort of thing.

Might be worth trying the cheapies.

I looked through my pics, but I couldn't find any metal pieces. If I get a chance in the next few days (between turkey and such), I'll try something.

Pretty sure I even used those bits on glass once just playing around.