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

Thin disc of aluminum sticking to endmill

O

Olo Manolo

Plastic
Joined
Jun 8, 2019
I'm cutting 1/8" sheet making some auto-parts with a lot of through holes. The issue I'm running into is a disc of aluminum getting stuck to the bottom (cutting edge) of the bit, so after it retracts and moves to the next hole, it has to puuuuush then POPs through the material like a punch instead of cutting into it. It happens using either 2 or 3 flute HSS or coated carbide. It happens even when I use a .3" or .5" ramp. I am using a 2 head fogbuster, sometimes it blows the disc off before the next hole, but its about 50/50. I'm running ~200IPM @ 18k and ~35IPM plunge.


Any advice or can anybody explain what is happening?

Thanks for your help,
Olo
 
Olo Manolo said:
I'm cutting 1/8" sheet making some auto-parts with a lot of through holes. The issue I'm running into is a disc of aluminum getting stuck to the bottom (cutting edge) of the bit, so after it retracts and moves to the next hole, it has to puuuuush then POPs through the material like a punch instead of cutting into it. It happens using either 2 or 3 flute HSS or coated carbide. It happens even when I use a .3" or .5" ramp. I am using a 2 head fogbuster, sometimes it blows the disc off before the next hole, but its about 50/50. I'm running ~200IPM @ 18k and ~35IPM plunge.


Any advice or can anybody explain what is happening?

Thanks for your help,
Olo
Click to expand...

.
aluminum sticking to edges especially at higher feed rates and coolant with not a lot of force is not uncommon.
.
that is your feed rates are not faster if you have to deal with problems caused by the high feed rates
 
Is this disc the size of the endmill?
Sort of a cap or plug that almost fits the tool or is it the size of the hole? (you say ramp so I'm guessing that you are interpolating)
What does the edge of the bottom of the hole (break through) look like with a magnifying glass?
Is it torn outwards in a area that matches the end mill dia?

Have you tried to reduce the ramp or feed just before you get to the bottom of the stock?
Bob
 
often going slower rpm and much slower feeds will help with slug sticking. if you ever ran a manual rotary broach drill in a magnetic base drill slug sticking is a lot less if you back off feed before breaking through.
 
Are you plunging these holes? I assume the issue is that the end of the end mill has a slight "dish" to it which results in the periphery of the disc being cut all the way through the material and it becomes stuck in the tool. Can you predrill these holes and finish to size with the end mill? Can you helical interpolate all the way to the bottom and then open up to size?

Edit: Guess I was a bit slow posting. A few people beat me to the punch!
 
35 ipm plunge what .2 depth thats .006 of min or .11 seconds ?? not sure the blink of a eye plunge rate saving you time if you got to stop and manually push slug stuck to end of mill off
 
It is a 'cap' that is the exact diameter of the bit, I'm routing out squarish holes. You can watch the plug going along for the ride while the bit is cutting out the shape, then sometimes the disc stays at the bottom, sometimes it sticks and goes on to the next hole.

I have tried plunging as slow as 15IPM with a .5" ramp, it still had the issue. I haven't tried slowing it down before the bottom of the stock though, I'm not sure that is something I can do in VCarve...
 
Plunging endmills went out of style at the same time as bell bottoms and hoola hoops. Ramp or helical entry can be pushed 5x as fast without the risk of loading up and endmill. If you gotta plunge, hit it with a 3 flute carbide drill at 300 IMP, then drop in your endmill.

I don't know about the rest of you dirtballs, but that we always referred to those funny little circle pieces at the end of an endmill or drill as China Hats. I saw one almost take a guys head off with a 2" spade drill.
 
If you are tool changing, bang through your plunge point with an undersized drill first.

If you are not tool changing, ramp in

If you cannot ramp in, ball endmill
 
I would definitely predrill a start hole so you don't have to plunge with your endmill. This effect is definitely coming from the shallow dish in the endmill and the soft material.
 
Guys- he replied that its 5052 aluminum- yea ramp it whatever but slow things down a whole bunch- and increase your coolant concentration. 5052 is gummy and not particularly happy about being milled- nothing at all like 6061 etc
 
The only problem there is that I'm fixing my sheet to MDF with CA glue for hold down, then after each set of parts i surface the MDF so i get several uses out of it. If i use a drill style bit it will run deeper into the MDF and I'll have to replace it a lot more often.. otherwise i agree this would fix my problem
 
How far into the wood are you cutting when you make the hole? However much you are facing off is how deep into the MDF you should be when profiling. That will help the cutter shed the aluminum.

Since the plunge is just an entry, change it to a ramp parallel to, and as long as the longest side of the cutout.

If you can't go slower than 18K, consider using a smaller diameter tool. The router bit is a good idea, at 18K rpm you should be hauling ass on the feedrate.
 
Vancbiker said:
For 1/8" 5052 sheet, I'd ditch the 2 or 3 flute endmill and use an Onsrud single flute router bit.
Click to expand...

I've not had much luck with single flute bits, plus slowing down enough to use one would greatly increase my cycle times and I'm running on a pretty small profit margin as it is.
 
You must log in or register to reply here.

Similar threads

R
Cutting discs for aluminum
Replies
1
Views
163
???
???
DeltaV
Need help with Okuma MC4 VAE, Parameters are lost. I need to re-install them.
2
Replies
24
Views
1K
DeltaV
DeltaV
U
Cutting tool for as-cast, Aluminum, dowel pin?
Replies
8
Views
606
LockNut
LockNut
Shiseiji
'54 Square Dial Sight Glass Disc is Permanent Party to the Headstock
Replies
11
Views
374
Shiseiji
Shiseiji
F
What is the most efficient way to cut a counterbore?
Replies
19
Views
1K
Garwood
G








 

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