What's new
What's new

Slotting tool recommendations

meowkat

Aluminum
Joined
Aug 18, 2013
Location
IL USA
I'm having a heck of a time getting good tool life doing some slotting around a circular profile in thin steel plate (0.130" thick). 5" diameter circle on each part.

I'm currently using:
https://www.mscdirect.com/product/details/78978020
(OSG 44700211 3/16 3fl high feed style)

OSG recommended a similar tool with flutes that have an angle to aid in chip evac: 447200113

But the tool life just isn't what I want, I'm fairly convinced the carbide that OSG thing is made of is some kind of mithril/vibranium but the edges are just about chowdered up and it's leaving some nasty burrs after ~45 parts.

I've broken so many traditional endmills trying to slot the circle of these plates I really need some good advice. The only other tool I have had luck with is a 3 flute roughing endmill from lakeshore carbide--I do a reasonably steep (for me) 7 degree ramp into a short slot (3/4 long) through the plates in about 10 places per part, trying that same recipe on the larger circle was just another broken tool.

So, if you were in my shoes and had to use a 3/16 endmill to slot circles in 0.130" thick plates, what tool would you use? :willy_nilly:
 
Are the slots going all the way through the sheet? Are there existing holes or slots you're starting in? 3 flute end mills are not center cutting. How rigid is your setup? You have a large area considering how thin the sheet is. Is it held tightly to avoid vibration? If not, consider two sided tape or a vacuum fixture. What kind of steel are you cutting? Both of those OSG endmills look like they are for hardened steel.
 
Odd suggestion but try an endmill more suited for hard materials, the edges will have more support behind them and if you use one with corner radii those will be protected too.
 
What material are you Machining?

R

A1011 plate, it shouldn't be hardened but it's pretty tough and hot rolled. The slots go all the way through, it's held down reasonably well for plate (I probably need to buy a cheap magnet and just mill the crap out of the top) and yes the tool is a hard milling category but it's also recommended for softer stuff too in the details.

I might just try the double sided tape.
 
Are the slots going all the way through the sheet? Are there existing holes or slots you're starting in? 3 flute end mills are not center cutting. How rigid is your setup? You have a large area considering how thin the sheet is. Is it held tightly to avoid vibration? If not, consider two sided tape or a vacuum fixture. What kind of steel are you cutting? Both of those OSG endmills look like they are for hardened steel.

Huh?? What are you buying/using?? :confused:

We use 3 flute endmills from .006-.500 and almost all of them are center cutting....
 
...So, if you were in my shoes and had to use a 3/16 endmill to slot circles in 0.130" thick plates, what tool would you use? :willy_nilly:
I don't understand why you picked a cutter with a 3/32" LOC to slot an 1/8" plate.

I'd use something like this:

Niagara N85590 | 3/16" Diameter x 3/16" Shank x 5/8" LOC x 2" OAL Right Hand Cut Center Cutting Single End Solid Carbide TiAlN Coating Square End Mill - All Industrial Tool Supply

Stone a radius on the corners, or buy the version with a corner radius. Choke it up in the collet, helical toolpath, a couple times around to depth should be easy-peasy. I think they make that cutter with a 3/8" LOC which would be even better...
 
heck no...why would you go backwards in technology?

Sounds like you are gripping that part in a a vise?

I would drill 4 hole in the corners and bolt it down to a fixture plate for that thin material. no more warping, no chatter, plenty of support...
 
heck no...why would you go backwards in technology?

Sounds like you are gripping that part in a a vise?

I would drill 4 hole in the corners and bolt it down to a fixture plate for that thin material. no more warping, no chatter, plenty of support...

I have it screwed down with 4 5/16-18 screws to a 1/2" steel plate on top of a pierson pallet. The double sided tape should tell me if it's lifting up and breaking the tools.
 
My calculator says 5000rpm and 29.4ipm. Thats what Id try... I doubt your part is lifting up any, I think the feed is just double what it should be.
 
I'm having a heck of a time getting good tool life doing some slotting around a circular profile in thin steel plate (0.130" thick). 5" diameter circle on each part.

I'm currently using:
https://www.mscdirect.com/product/details/78978020
(OSG 44700211 3/16 3fl high feed style)

OSG recommended a similar tool with flutes that have an angle to aid in chip evac: 447200113

But the tool life just isn't what I want

So, if you were in my shoes and had to use a 3/16 endmill to slot circles in 0.130" thick plates, what tool would you use? :willy_nilly:
I wouldn't use a 3/16 tool, I'd use a 2/16 one and spiral path it.
 
Kids!!!

It's not backwards if it works. HSS is slower than Carbide. It's also tougher.

R
Agree in a sense. If you suffer tool breakage continuously with carbide the cycle time is pointless if you spend the same time replacing tools. Expensive tools.

If mass production on the other hand take your time figuring shit out.
 
Small update, tried the niagara and got lots of chatter, tried a guhring diver and got a little bit of chatter and then it exploded doing a straight plunge as advertised, tried a kennametal Harvi 1 HPHV and it took the same cut as the guhring diver did but quietly and hasn't broken yet. Should turn this job from low paid into easy money.

I think the kennametal is a great tool so far.
 
Perhaps a left helix, right hand cut end mill would tend to push down on the part to push it to have more support and less chatter..

Could a ball nose probe/finger set just above/near and touching the part and travel about on the part as you are milling so also to reduce chatter with using your existing cutter...probe carbide/steel even nylon..

Seems like chatter may be some/much of the short tool life.

https://www.homedepot.com/p/Yonico-...-4-in-Shank-CNC-Router-Bit-32313-SC/306082371

Harvey Tool - Carbide Plastic Cutting End Mills - Square Downcut Single Flute


4 Flute Square Downcut End Mills - AlTiN Coated - MariTool

*Agree you don't need a single flute or a plastic end mill..double or 3 flute and left helix, right hand cut would be good.

The fixture having support (touching) just under the part and along the slot being machined..
 








 
Back
Top