What's new
What's new

360 brass...

Solar71

Titanium
Joined
Mar 24, 2005
Location
Hermosa Beach California
Hey all...
Im not sure how its written...
360 or maybe 3-60 or something like that...

I am getting 2 x 20 foot bars of 2.5 inch diameter brass...

I want to machine it at a high speed... and at high feeds too...

I have never cut anything brass before...
This will be Lathe work...

I will be using an insert drill first...
Then turning it down on the ID and OD with all kinds of radii and grooves...

Now... Here is the question...
What do you guys think about using coolent for cutting faster and faster ?

Is coolent bad when mixed with brass ?
None of the guys at work use coolent while cutting brass... But i have watched them cut brass... and they always cut it slow...

These parts i am making are called Thrust plates... They work with the ball gears i just finished making...

I will be making close to 400 units...
And i want to make these as fast as possible...

I have seen the other cnc machinist guys make this same part... His programs runs for (ABOUT) 8 minutes... I would really like to shoot for 4 minutes or less per unit...

This is sort of a challenge for me...
It makes the machining and programming more enjoyable if i have a "time" goal to shoot for...

So ...

Can i use coolent to go faster ?
Or do i just run it dry ?

What are your thoughts on this 360 ( 3-60 ) brass stuff ?

thanks
 
I kind of have a love/hate thing with 360 Brass:
-Love it because it looks pretty.
-Hate it because of the chip mess. The harder you go at it, the farther the chips travel. And they get in everywhere they shouldn't and they are sharp little suckers to boot.

Anyways, another secret that may not be secret, but negative rake inserts work okay, but brass likes a very sharp cutting edge, or it tends to smear and the surface is not pretty. Even the slightly honed edge of a negative rake insert is too dull to do a good job.

Since I cannot be bothered to order up a special box of inserts, I take and grind the top of the chipbreaker off so the top face/leading edge of the insert is smooth for as deep as my depth of cut will be. This leaves a very sharp edge, and the finish is good.

Because I hate the chips spraying all over the place, I often fabricate a chip deflector to go under the top clamp of the toolholder insert pocket, and use this to try to direct the flow of chips somewhat. An extreme depth of cut at a fine feed will also give some measure of chip control, without taking too awful long to do the roughing.

Coolant is optional, although there is a lot of heat released in cutting that you would otherwise have to allow for shrinkage as the part cools down.
 
it sounds like you guy are saying coolent is optional..

i CAN use it... but i dont HAVE to...

Am i correct ?

If i do use coolent... what are the advantages/dissadvantages of using coolent or NOT using it ???

Seems like i should be abble to ge much faster WITH coolent...

But is this true ?

PS : the other guys at my work that machine brass in the CNC lathe are always lining the inside of the machine with cardboard... So they cant use coolent... Seems like they dont want the brass getting into the machine AT ALL...

Do i need to worry about this ?
If the chips stay away from the weys will i be ok ?

PSS : is there any way to make the brass chips Larger ? So they dont get into everything ?

PSSS : I am planning on turning the brass at .0625 DOC (.125 dia) per pass... At F.010 and at about 1,200 rpm Roughing...

And F.005 S1,800 finishing...

Does this sound ok ?

ME consoltant suggested MUCH MUCH faster... but that scares me... HAHAHAHA
 
Some coolants, maybe with sulfur, will stain brass, and other copper alloys. So that may be one reason to avoid using it. If the parts will be plated it doesn't matter anyway.

DOC? I don't know, but even a small engine lathe is happy at 1/4" or better.
 
You lucky dog,
You are turning the easiest brass there is. They don't call it free cutting brass for nothing. I will agree that 360 brass likes sharp tools. I personally use T-15 positive rake inserts from Arthur R. Warner in Latrobe PA USA. Just call and talk to Mike Warner. He will supply you with inserts that will make 360 look like it was polished. If you go elsewhere, make sure you get positive rake inserts.

I agree that the chips are sharp little buggers. Fortunately they are not as damaging as ferrous chips. After all they are about 2.5 to 3.7 percent lead.

Coolant will make life easier for you. I suggest a flood coolant first.

Speed is what you can give. Treat this stuff like 2011 aluminum, only smoother. Feeds are only dependent on the finish you want, and the tool you are using. A positive rake tool gives smooth and shiny finishes, but negative tools that are super sharp will give almost as good results. Depth of cut is determined on material cross section, overhang, and your nerves. The chips can look like water coming from a hose and the finish will still be pretty impressive. Be daring and play with the variables. Each setup will be unique for 360. Mike Warner can give you hard numbers for specific inserts.

Good luck and keep er' flying.
 
Solar

You can go MUCH deeper than .065 DOC. Your surface speed may be more dependent on how much you want to spin with a 2.5" bar in the spindle, make sure to limit the RPM to something sane. Feedrate is almost mute, .01 - .012 - .014 or heck, you can practically cut it in rapid.
Yes, chips will go all over the place, but then again they are just chips that will eventually end up in the chip-tray of the machine. They are smaller , almost powder like sometimes but it's not bad for the machine though.
Bob stated it is more abrasive than AL, I did not find that at all. Just finished rough turning and finish boring 200 feet worth of the stuff, and did not change inserts or offsets, the last part looks and measures just like the first one.
Now on that same note I have a question. My second op on this part is exactly 10 seconds long, as it is simply wiping a continuous contour on the OD. I'd like to do away with opening and closing the door and having coolant all over my hands to make it slippery. BUT, I need an eventual almost mirror finish, so I need something to help carrying stray chips away that may scuff the surface. Do you guys recommend some type of oil, WD40 or whatever else to just rub on the tip of the tool or the part very lightly?
 
Coolant is optional, although there is a lot of heat released in cutting that you would otherwise have to allow for shrinkage as the part cools down.
If i do use coolent... what are the advantages/dissadvantages of using coolent or NOT using it ???
Hu is saying that if you run hard and don't use coolant, your parts might not mike the same when the customer gets them as they did when you ran them.
 
Thanks you guys...

So i think i will flood coolent the parts...

Cut massive DOC!!!
and Spin Massive RPM!!!

I hope this is as easy as you guys make it sound...

thanks again for all the tips...
unfortunately, i know my boss... and he will not buy special inserts just for cutting brass...
He will give me those black, cheap, uncoated inserts... But thats ok if its as easy to machine as you say...

Unfortunately they wont be the "PERFECT" inserts... so i may need to go a little slower then optimal... but thats cool...

I think, with a little luck i will cut unit cycle times in half, compaired to the other machinists... So its all good...

thanks again
 
i second the opinion that 360 brass is easy on tools. we used to run 10k pc lots of brass parts and never had to change tools and made only the slightest adjustments to offsets. run the rpm as high as is feasible (vibration will be an issue if running from bar) and feed it hard. not running coolant has 1 benefit, cleaner chips for the scrap guy.
 
There will not be any bar stock in the spindle...

MY through hole for the spindle is only 2.062
and the material is 2.500
So it will be cut in a saw first... then i will get about .500 inch units...

So not too much material in the spindle at any one time...
 
when i'm drinking coffee i'm extra smart...

tell your boss that you want all the money from the brass chips (you do sell your valuable chips don't you?) to buy tooling with. you will be surprised at how much you can get for clean brass. do not let it mix with other metals. make sure your machine is very clean (free of steel, stainless, etc.) before you run the brass and keep the chips in a drum. all he will be out is the scrap money and you will get some more tooling.
 
360 Brass has a machinability rating of 100%. You can pretty much machine with anything you have and get good results. Better tooling will give better results in time and finish.

I use coolant mostly to move the chips and hold tolerances due to heat buildup. Sulfur based coolants will stain parts and will need to be washed.

Word of caution, sharp tools grab in brass. Especially drills. A drill following a pilot hole will act like a screw. A poor setup will yank a part from your hand, vise, fixture, chuck etc.
 
"""
Word of caution, sharp tools grab in brass. Especially drills. A drill following a pilot hole will act like a screw.
"""

Ouch!! Where were you BEFORE I've learned that painful lesson?
 
Good advice from SIM. Drilling brass can be a little hairy. Stoning a small flat (.01") on the cutting edge of the drill will keep the grabbing down to a minimum. Another chip control device can be made by positioning a brush on the cutting tool to keep the sharp little devils from getting air born.

ARB
 
Good advice from ARB on SIM's advice :D

At the risk of riling up Charlie Biler ;) , I do not advise working brass or bronze with positive rake tools. Neutral rake (and no chipbreaker required) is best to avoid nasty accidents, as well as improve the exit of a drill through a hole.
 
I will be using an insert drill...
no a twist drill...

Do i still need to worry about the drill pulling on the material?

I will be drilling a 1.312 hole at about 1,200 rpm and at about f.003 or so...

My final ID will be 1.353

thanks
 
Solar,
I think it depends on how close the chipbreaker is to the edge, and how hard you are feeding it.
If you feed it fast enough that the chip goes over the edge lip and down into the chipbreaker geometry on top of the insert, then that effectively creates a positive rake action, that might tend to pull the work onto the drill.

At a slow feedrate, if you watch the drill behaviour as it begins to cut, it should cut steadily. If it cuts/stops/cuts/stops then the drill is wanting to hog into the work.

Again, inserts that you might use for drilling steel will have honed edges, which are honed so that they are able to stand up to the tough cutting. But, for brass, the honed edge is likely a bit too dull. Inserts with a smooth flat top, and perpendicular to the work will work best, IMO. You can buy plain grades like that, I think. But, I would just take some slightly used inserts over to the diamond wheel and grind the chipbreaker off flush near the cutting edge, to create my own instant brass cutting insert.
 








 
Back
Top