Cutting brass vs aluminum questions

Mud · Nov 12, 2020

Rookie questions from an old fart here. A customer has asked us to make 2 sample parts from brass, otherwise identical to the parts we make for him out of aluminum. The total amount of brass chips I've made in 50 years would be unlikely to fill a cigar box, about all I know is the warnings I've read about it grabbing drills during drilling. Can you give me a little guidance here?

Part is 6" dia X .625 thick, involves a little milling around the OD and face of the blank for preparation, drilling 6 .875 through holes and 6 .192 through holes, counterboring those 12 holes, then turning and face grooving one side, flipping and turning the other side, then drilling and tappng a 3/8-24 hole in the center. We've done thousands of these on 6061-T6 and have the process pretty much optimized for aluminum with insert mills and drills and a couple HSS tools in the VMC, and CNMP inserts and Iscar groovers in the lathe. Can I run the same speeds and feeds and coolant on brass? Do I need to reduce speed and feed for brass? Do I need different tools altogether? Customer is sending 2 pcs of material and expects 2 good parts in return, seems it's pretty expensive. What trouble can I get into here? Appearance is critical on the finished parts. The .192 holes are counterbored to .625 dia, the bottom needs to be nice, and the turned surfaces need to be nice. No SF requirement, just good looking, possibly polished in use.

EmGo · Nov 12, 2020

Brass is easy, pretend it's aluminum except you get teensy little sliver chips that fly all over and stick in your body.

BRONZE is a bitch

Kyle Smith · Nov 12, 2020

I'd run it exactly like the 6061 version, maybe back off the feed and RPMS 20% on the first one to see how it goes. If it's 360 brass it is pretty forgiving and easy to get nice finishes. Drills tend to grab when used in a free moving quill or hand drill. In a rigid VMC I don't have any issues with grabbing. If you do, it doesn't take much of a land on the drill to eliminate the hook and fix the issue.

L Vanice · Nov 12, 2020

There are many different material specs for brass, so it would be good to know which one the customer has supplied. C36000 is the easiest to machine. In general, coolant is not required for at least some grades. In general, cutting tools need neutral (zero degree) back and side rake for best results. Surface speed can be the same as for aluminum. Feed may depend upon the tool geometry.

Sounds like your turning tools, drill bits and counterbores may need new geometry. The special tap might still work OK if you turn it by hand just for two parts.

If he gives you some pretty yellow chunks of aluminum bronze instead of free machining brass, refuse to touch them.

Larry

crossthread · Nov 12, 2020

You might want/need to drubb your drills. I always have when drilling deep into brass. There is a lot of information on how to do this. Google "drubbing drills". The purpose is to keep the drill from grabbing. Works very well.

Limy Sami · Nov 12, 2020

What they said ...and save the chips

P.S. Just a wee reminder that Brass is much much heavier than Alu, ..........and worth more in scrap ...............and I don't think I need to draw a picture

Mike1974 · Nov 12, 2020

I program the exact same tools, speeds, and feeds for brass and aluminum. Our machines are limited on rpm, so I can't hit the SFM on either unless I get to bigger tools than we typically use.

L Vanice · Nov 12, 2020

crossthread said:
You might want/need to drubb your drills. I always have when drilling deep into brass. There is a lot of information on how to do this. Google "drubbing drills". The purpose is to keep the drill from grabbing. Works very well.

You get better results if you search "dubbing drills." It is a term for changing the back rake of the cutting edge to zero degrees.

"Dubbing" Drill Bits?

Larry

DDoug · Nov 12, 2020

On the (6) .875 dia. holes (thru .625" thick ?) I would switch to an endmill and circular interpolate, no worries about catching & dubbing correctly.

Mud · Nov 12, 2020

Drubbing the 7/8" drill will ruin an expensive Sumitomo carbide insert. Reprogramming to interpolate will eat up a bunch of time we don't want to spend on 2 parts. How likely is the drill to grab the blank and pull it up out of the .100 deep soft jaws if we just slow the feed? Can go infinitely slow just by turning the override knob.

L Vanice · Nov 12, 2020

Mud said:
Drubbing the 7/8" drill will ruin an expensive Sumitomo carbide insert. Reprogramming to interpolate will eat up a bunch of time we don't want to spend on 2 parts. How likely is the drill to grab the blank and pull it up out of the .100 deep soft jaws if we just slow the feed? Can go infinitely slow just by turning the override knob.

You must be charging for those two parts and allowing for time and tooling, so why not get a cheap HS 7/8" drill bit with 1/2" shank and dub it? One tenth of an inch into the vise jaws does not sound very secure. Remember, you do not have spare blanks.

Larry

david n · Nov 12, 2020

Use the same tooling............just tweak feeds 'n speeds.............................

crossthread · Nov 12, 2020

You are correct sir. It is dubbing not drubbing. I have prostituted myself to spell check again.

Limy Sami · Nov 12, 2020

yes Drubbing means a beating or thrashing, drubbing - Google Search

mhajicek · Nov 12, 2020

Use the exact same tooling and program, run it at 80% for safety, and be done.

Phil in Montana · Nov 12, 2020

Just use sharp tools, everything will work out good...Phil

TheBigLebowski · Nov 12, 2020

What kind of brass? It machines easily but, depending on the exact type of brass and who supplied it, there is potential for some really nasty internal stress relief after machining. Stress relieving might be required.

I had a smallish brass job that I ran this spring (20 or so pieces). The material was 1-1/8 square brass stock that I got from Alro. The material was terrible, lots of warping for cuts that were pretty minor. I scrapped 10 or so parts because I left 0.005 per side for grind and they moved 0.020+

From what I have read, I am not the only one who has had issues with brass from alro.

Mtndew · Nov 13, 2020

Mud said:
How likely is the drill to grab the blank and pull it up out of the .100 deep soft jaws if we just slow the feed? Can go infinitely slow just by turning the override knob.

Unless you tightened the vise with your feet, you'll be fine.
Grabbing the drill is usually done when you're using a Bridgeport and it has potential to suck the quill down when breaking thru.
If this is a cnc, and you're holding it the same way you'd hold the aluminum parts you'll be fine.
You can use air blast instead of coolant if you wish. Brass is the delrin of metals. So nice to machine.

Mcgyver · Nov 13, 2020

what Brass? they can vary widely in alloy and hardness, but half hard 360 brass (probably the most common bar stock) is one of the nicest to machine materials. Speeds can be up 2x steel.

I'm surprised at all the "use the same tooling" comments. Machining brass works best with a really sharp cutter, hss imo is best. I keep separate files for brass and use freshly sharpened endmills as once used on a steel they are sub-optimal on brass. Regular end mills work fine, but for turning and drill, zero rake is the order of the day. zero rake makes a BIG difference in finish and not having a tool jam.

Mike1974 · Nov 13, 2020

Mcgyver said:
what Brass? they can vary widely in alloy and hardness, but half hard 360 brass (probably the most common bar stock) is one of the nicest to machine materials. Speeds can be up 2x steel.

I'm surprised at all the "use the same tooling" comments. Machining brass works best with a really sharp cutter, hss imo is best. I keep separate files for brass and use freshly sharpened endmills as once used on a steel they are sub-optimal on brass. Regular end mills work fine, but for turning and drill, zero rake is the order of the day. zero rake makes a BIG difference in finish and not having a tool jam.

We cut half hard brass nearly daily. We use the same tools as we use on our aluminum parts. It might not be the *best* but it cuts all day every day just fine. We are typically holding onto .12" or less in vise jaws, so "grip and rip" is not really our forte'. We do have some jobs that run in talon grips, but that's usually a "special" job.

Cutting brass vs aluminum questions

Diamond

Diamond

Stainless

Diamond

Titanium

Diamond

Diamond

Diamond

Diamond

Diamond

Diamond

Diamond

Titanium

Diamond

Diamond

Stainless

Aluminum

Diamond

Diamond

Diamond

Similar threads