What's new
What's new
By:
Advanced search…

Machining copper

L

Lazybone

Plastic
Joined
Oct 5, 2003
Location
Goodyear,Arizona USA
What speed would work best when drill a 7/16 hole 4.0 deep hole in copper material always have drill breaking problem. I am currently using a pecking cycle going 1000rpm , .075 per peck,.100retract , feedrate of 4. using a Fadal mill. Any suggestions for better results ?
Thanks
 
Coolant type? Copper alloy and condition? 90% of problems machining copper in my experiance have been lube problems. We used to use Tapmatic #2 tapping fluid for all copper machining in the late 70's. Dont know if they still make it though. Polished flute drills gave us the best results, used with fluid of course!
 
What type of copper?

Some types of copper have a machinability rating in the cellar. Copper expands at the tool and tends to pinch and hold and does not have very good lube qualities of its own.

gg's advice is good.
 
For a start, your in to much of a hurry,

Start with a Split Point Drill at 40Ft/Min ... 360 RPM
Feed at .003 to .005 in/rev
FULL retract after a .100 depth of feeding
Make sure the drill is clean and there are no chips in the hole as the drill will not like re cutting them. If that goes well, increase the .100 feed depth to .150

As said, plenty of coolant, I would not use tapping fluid unless your doing this on a manual drill press, and I am guessing your not.

You may need a Drill made by Guhring
 
In the "Bedside Reader", Guy Lautard says that MILK is the best lube/coolant for machining copper.
I haven't tried it, personally. :confused:
 
Through tool coolant is the ideal way but it doesn't sound like you have that option.

I agree with Gary, 1,000rpm is way too fast. 300-400ish RPM is far better, you can experiment a little. Full retract is mandatory, copper chips are sticky and will not want to leave the hole otherwise. Try finding a coolant more suitable for copper, and/or use a stronger mixture for more lubricity. Keep in mind many coolants will stain copper if they are not compatable or used in too strong a mixture. And use lots of coolant but be careful it's not flushing chips back into the hole on retracts, they won't recut like many other alloys will, they just smear back into the parent material, burnish the drill tip, and next thing you know you're digging out bits of HSS. Chip evacuation is probably one of your biggest problems going. Also polish the snot out of the inside of the drill flutes in the cutting area. Copper likes to stick to the cutting face and cause all kinds of problems.

Best of luck, I don't envy you! I think copper is probably on the bottom of every machinists fun scale ;)
 
So does this mean you can use yogurt for tapping? And the all important question... With or without fruit on the bottom?
 
Here is some code from drilling 110 copper that I did a few years ago. Used PTD EZ or QC style drills with TiN coating and water soluble coolant. If the drill starts squeaking it is time to change it, right away. Hope this is helpful.


(1/8 EZ JOB)
T4S2100M6
G83Z-1.16R0Q0.106F3.8


(1/8 EZ TAPER)
T5S2000M6
:0024
G81Z-1.33R-1.13G98F3.8
G81Z-1.47R-1.3
G81Z-1.61R-1.47
G81Z-1.72R-1.57
G81Z-1.83R-1.7
G81Z-1.94R-1.8
G0Z0G98
G0M99

(3/8 EZ JOBBER TIN)
T8S850M6
G83Z-1.8Q0.37F5.

(3/8 EZ JOBBER TIN)
T9S750M6
G83G98Z-3.2R-1.7Q0.31F4.5
 
I make copper buss bars out of c110 copper. I start at 150-200 sfpm and .003-.006 ipr depending on the drill diameter. This is 1310 rpm (150 sfpm) and 7.86 ipm (.006 ipr). I use HSS drills with an 118 deg point or 135 degree split point. Make sure your tooling is sharp. I don't like to peck drill unless it's a deep hole, which yours is. I wouldn't take such small pecks though, I'd drill the first inch then peck every half inch or quarter inch when you get towards the bottom of the hole. I use rustlick ultracut 255 coolant at a 10:1 ratio. I use this for milling, drilling, and tapping. I don't think copper is to hard to machine. It's basically like aluminum except a little gummier and a little tougher. Besides it's nice to take the chips back in to be recycled
Good luck.
 
your problem is that the drill is being sucked in by the copper chip,instead of having a positivve rake on the drill flute,you need no rake.not a positive not a negative,just a flat 90 degree on the tip of the drill.it may suprise you,try it you will like it.that is onthe cutting edge,which is alwys a positive rake.i have had the same problem with brass and that type of material in the past,by regringing the cutting edge i had a lot better results. bill
 
For what another opinion is worth, I do a job where I drill two 7/16 holes 5" deep in each piece, which is copper. I do them on a bridgeport and have to peck drill .050 to .100 and need to fully retract the drill. In my case, the material is 7/8 by 1-3/4 by 6 and the heat from drilling causes the piece to grab the drill, hence the peck drilling and full retraction. Also need to keep it as cool as possible. Now as I said, this is done on a manual machine but I tried using a negative rake tool but I found that a new or newly sharpened drill does the job best for me. Good luck!
Bill
P.S. As previously stated, save them chips!
 
Copper,I enjoy the few jobs I make out of it. I use sharp ( honed edge ) tooling and set my speeds and feeds on the conservative side. I can always speed it up if need be. Lubricant of choice is Non Detergent Motor oil,use plenty.
Saw the oil first used by one of the best machinist I have known. Hope this helps.
 
I found that when boring copper or brass, its actually better to dull your drill bit with a hone, that way its not so grabby.
 
You must log in or register to reply here.

Similar threads

E
Need help with tooling, specifically drill
Replies
15
Views
1K
Scruffy887
S
M
walking drills and pecking cycles
Replies
6
Views
559
madmachinst
M
I
drilling delrin without packing chips on the drill
2
Replies
39
Views
2K
triumph406
triumph406
K
Drilling in 303
Replies
12
Views
1K
specfab
S
3
Deep hole threading? 2x one shot or peck tap?
Replies
7
Views
689
Matt G
M








 

ABOUT PRACTICAL MACHINIST

With more than 10.6 million unique visitors over the last year, Practical Machinist is the most visited site for metalworking professionals. Practical Machinist is the easiest way to learn new techniques, get answers quickly and discuss common challenges with your peers. Register for the world’s largest manufacturing technology forum for free today to stay in the know.

Learn more about us.

STAY CONNECTED

Facebook Instagram YouTube LinkedIn Pinterest Twitter Tiktok

Register Become a forum member. Register today.

Sign Up Sign up for our e-newsletter.

© 2024 Copyright Practicalmachinist.com. All Rights reserved.

Back
Top