Machining Brass - Bits, Speeds?

[John TenEyck]

I'd like to machine some brass logo inlays. I've machined a little aluminum on my CNC w/o issue. I used a 0-flute upcut bit for pocketing and a V-bit for some chamfers, both with very conservative speeds and feeds. Can I use the same tooling, etc for brass, or ? Thanks for any input.

John

[Gary Campbell]

John...
When in doubt, look up your material on the Onsrud catalog or website. They will always have the right tool for the job. That said, there often is a less expensive bit or brand that will do the job well. Often, but not always. BTW, brass should cut easier than aluminum with your Oflute bit.

[John TenEyck]

Thanks Gary. I found a list from SpeTools, who I use most of the time. Many of the same bits I use for cutting wood can be used for brass, at much lower speeds but surprisingly high DOC, same as for wood, actually. Anyway, the bit manufacturers have recommendations for many materials, including brass. I have some C360 I think it is bar stock arriving today and will give it a go.

John

[Robert L Stewart]

John,
You will enjoy working with brass. These pieces are 2.2 x 3.5 x .125 thick. Each letter is .42 wide.
Profiled 262 pieces (360)with 1 standard .25 diam. carbide bit. The pocket and letters done with a .030 EM, nothing special.

498078

[John TenEyck]

Thanks for your input, Robert. That looks great. How did you get the texture in the recess, grit blasting or with the CNC?

John

[Robert L Stewart]

John,
Bead blasting

[John TenEyck]

John,
Bead blasting

I really like how that made it look. Thanks.

John

[John TenEyck]

Well that was interesting. I broke a new O-flute bit using SpeTools' recommended speeds, feeds and doc for brass, and then another at half the speed, but still the same doc, which I should never have used. I downloaded Whiteside's bit catalog into V-Carve Pro to see what they recommended for a similar bit. Even more aggressive settings. It seems unreasonable to me that you can use a 0.125" doc with a 1/8" bit (I don't even do that in wood), and then run it at 60 ipm per SpeTools or 160 ipm per Whiteside. I think I used a doc of 0.007" with a speed of maybe 30 ipm when I cut the aluminum. I'm going back to similar settings with the brass.

John

[Robert L Stewart]

John,

No luck finding my cut settings for the above posted pic of .125 thick 360 brass. Seems like .005 doc at 40 ipm is about right. I usually mill alum the same but at 60 to 80 ipm.

I had an order cutting 500 pcs of .032 x 3.625 x 5.875 brass. Using an O flute .08 doc, 35 fr. 8.0 pr. I bit did the deed. Another order for 5500 pcs of .060 alum with same settings.
No issues or lube needed.

Robert

[Jim Becker]

John, IMHO, there's no way you're going to get .125" DOC in non-ferrous metal with the kinds of machines we run. With wood? yea. Metal...nope. So yes, stick with the "manny passes" technique to both preserve the tool and insure there's no vibration and excessive heat generated.

[Carl Beckett]

I agree with the others on limited DOC. In fact, I dont believe I have run the feeds/speeds from tooling 'recommendation' charts ever. Others maybe have better luck, but always 'too much' or 'too fast'.

(and ya I was a machinist in my early life years ago - hobby CNC is not the same)

I generally run a test pass and look at finish left, but also LISTEN. The sound can tell a lot about how the system is performing.

[Michael Burnside]

For brass I usually target 0.003" chipload with a DOC of 1/64-1/32" with a 1/8" bit. I'm always thinking chipload. You can go conservative DOC but if your chipload is too low you'll dull the bit or break it, especially as you try to increase DOC. Not because you're moving too fast, but because a low chipload will heat the bit and weaken it.

Usually for wood I do DOC = diameter (more for compression bit) but soft metals it's a /4 or /8 the diameter at the proper chipload for the material. I feel sometimes the metal numbers assume some assistance with machining fluid?

[John TenEyck]

Another learning experience yesterday. I tried what I thought was a doc of 0.006" at 30 ipm on a 1/8 O-flute bit. The doc looked much greater when it was running, though, and after a couple of minutes the bit broke. I checked the tool parameters again and found I had somehow entered. 0.060". So I know that's too agressive, too. Next time, I'm trying 0.007" which I know works in aluminum. Oh, the chipload calculates at 0.0025. Gotta order some new bits first, though.

John

[Michael Burnside]

Been there, done that. A couple of weeks ago I burned through two bits because I screwed up the chipload and was spinning too fast. After burning/breaking two bits I looked and realized instead of 0.01 I was closer to 0.001 chipload. Some people say "listen" but honestly with ear protection and the dust collector going I prefer to look at the chips. In my case I was making powder LOL!

[David Kenagy]

I broke three Amana single-flute cutters on brass sheet (clock faces). When I asked Amana for advice they engaged their engineers (so I assume the advice is valid). Some lessons learned:

- If the cutter tip is very small, the movement due to rotation is very, very small. To make that work better, the rotation speed has to be high. Amana recommended 30k for a cutter with a 0.005” tip. (My spindle only goes to 24k).
- That small tip doesn’t remove much brass at a time. So travel across the surface (IPM) has to be extremely slow, or “you’ll scrape your tip off”. For me, that’s about 6 IPM.
- Apply the above to depth of cut. I use 0.003 to 0.006.
- Brass alloys differ. 260 half-hard is the best I could get (in sheets). 360 is better for machining, but mostly sold in thicker forms.

But the biggest lesson: brass dust gets to places you didn’t realize. My cyclone leaves a dust-free table. But when an expensive spindle overheated, the manufacturer found brass dust in the bearings. If you’re going to machine brass, you should use a disposable router or put an air seal on your spindle.

[John TenEyck]

Thanks for that info. David. My continuing disappointing results is confirming the data you reported. I broke all three zero flute bits I had, even at 0.006" doc. The feed rate must still be too high for the 1/8" diameter bit. Can't remember for sure but I think it was around 25 ipm. I ordered 360 brass but have no way of knowing if that's what I actually received. I have no trouble machining aluminum, but brass is presenting much more of a challenge. I've put it on the shelf for now as I need to get some work done.

John

[Grant Wilkinson]

FWIW, I cut brass dog tags with my Sienci Long Mill. The brass was 1/8" thick. I used a 1/8" o-flute bit. Depth of cut was .007", feed rate was 20 ipm and router speed was as low as I could get the Makita router, which I believe is 10,000 rpm. I didn't have many to do, so I stood there and blew air from a canned air to keep things cool. (I had done that successfully before with aluminum.). No broken bits and a happy vets office.

[John TenEyck]

Thanks Grant. Those parameters are about where I'm headed when I get some new bits.

John