Cutter to machine hardened steel?

[Bob W.]

I need a cutter to machine A2 at RC60. I need something in 3/8" diameter with a ~2.25" reach. Any suggestions?

 

Thanks,

Bob

[Bruce Caulley]

I usually use Garr for solid carbide, but don't do much that hardness. Give your tool rep a call would be the best bet.

 

Bruce

[Gordy Programmer]

I use a lot of Garr tooling also, but only up to RC40 or so. If we get up to RC60 we will wire or Cedm the part.

 

Gordy

[strabe]

YG-1 makes endmills designed to cut up to Rc 70. It's thier X5070 line, although I have not personally used them.

 

Are you side milling or slot milling? More info needed to help you further.

 

Ken

[Chipmakr]

What type of machining do you need to do side milling, slotting, surfacing? How much stock do you need to remove? What kind of machine, RPM range, and toolholding will you be using? If you can give more information I can give you a better answer.

 

We cut alot of 55-62 steel around here. As far as which tool would but best for you, it really depends on what you are trying to do and what you are trying to do it with.

 

Not trying to be difficult, but there is no use suggesting a expensive tool that mighht work fine in a good setup only to have you order it try to cut with too much runout and blow up tool.

The would not benifit anyone.

 

[ 07-30-2009, 10:26 AM: Message edited by: Chipmakr ]

[Tim Simmermon]

SGS Power Carb

 

I've used these before in 4140 @ 55 Rc. Beat the snot out of YG-1 X-Power. Ran 4x as fast and the cutter lasted twice as long.

 

[Bob W.]

I am side milling to create a sharp vertical step where there is currently a radius. Very little material is being removed (~.040" side cut, .1" deep) but the resulting corner needs to be sharp, so no radiused end mills. I machined these parts and accidentaly left out this final operation and didn't realize it until the parts were heat treated so this is a one time deal, though there are 220 parts. The machine is a Haas.

[Hardmill]

A sharp mill will work best

read this from MMS Online :

Solutions For Hard Milling: Cutting Tools Transcript

 

When cutting 60 Rockwell, be aware that there are cutters specifically designed for this material. Using anything less will cause unwanted results. If you want to get to a bench-free surface finish and want that part to have an accuracy based on being able to shoot a mold, you need to be mindful of the tol

inMotion Transcript from: Modern Machine Shop

Posted on: 8/28/2008

 

When cutting 60 Rockwell, be aware that there are cutters specifically designed for this material. Using anything less will cause unwanted results.

 

If you want to get to a bench-free surface finish and want that part to have an accuracy based on being able to shoot a mold, you need to be mindful of the tolerance specifications of the cutter. For instance, if I'm cutting half of my parts to zero and half of my part to negative stock and I want to make sure that on my parting surfaces are closing. I must pay attention to the tolerances of the tool to make sure this will happen without bench-time.

 

Geometry also plays a part in tools designed for 60+ Rockwell. Because the tools are designed for hardened materials, their cutting angles vary according to the manufacturer's testing. There are ballnose endmills like the OSG SHP series that has a 15 degree angle on the cutting edge around the cutting flute. There is also what is known as a true four flute ballnose endmill that has 30 degrees on the cutting angle. Kind of goes against the 15 degrees and the two flute ballnosed endmill but because this is a four flute and it is a true four flute which means that the cutting edge comes all the way to the center this tool is actually 30 degrees. A high helix angle or a 45 degrees doing a six fluted cutter which would have a 45 degree angle on it going long depth but shallow step over or shallow radial step over. Choose a tool that fits the specifications you are looking to achieve in your hard milling application, keeping in mind that there are several options out there.

 

In order to allow for decent tool life in such hard materials, most manufacturers add a coating to their tools. A Hitachi TH coated endmill or a ballnose endmill is an example. The coating makes the tool a gold color. Other examples include OSG with the Max series as well as their SHP series, Mitsubishi has Impact Miracle, NS has Mugen, Polkom has PVAT, and Union Tool has what they call the Hard Max coating. All are excellent for 60+ Rockwell applications.

 

~~~~~~~~~~~~~~~~~~~~~~~~~

Look into mitsubishi or Union tools.

The Higher end OSG cutters will get er done too.

 

Email me if you need help

 

 

PEACE

[MotorCityMinion]

IMO:

Depends on your tolerance. Tight tolerance?, the Haas won't do it consistently with that quantity. The cutters will die too fast. Think twice about not using a radiused emill. I'd at least hit it with a radiused tool 1st, then come back with the sharp to finish it. Hardened steel and sharp corners on a e-mill don't get it when you have to finish a bottom surface with the tool. That quantity of 220 parts justifies using 2 tools. Also note that if all your doing is removing the stock at the bottom, relieve the E-mill as much as possible to reduce tool pressure. That Dia. to length ratio is pretty nasty also. Resist the temptation to baby it and 1 pass it with each tool. Good luck.

[mchin-pilot]

It is possible, and not too difficult at all.

Dont be afraid , job can be done.

Every cutter company has Hard milling cutter range ( TiAlN coated),contact your local suppliers.

Do not use coolant.

Use Air blast.

Has to have the Hard milling strategy(Step overs,Step downs,F,S)

[F800R]

Check out Seco's Jabro line of solid carbide. Call Eric Gardner 877.908.3726 or [email protected].

 

This guy is good.

 

K

[Chipmakr]

KKlaver has a good suggestion there.

 

We use Jabro here when the difficulty of the job requires it. They make really good tools and based on my experience this would be the best solution for you. The JH170 series will work very well. Depending on the diameter this tool can have as large as a .007" corner chamfer. If you start with a sharp cornered end mill you will not have a sharp corner for very long anyway so I would just go ahead and start with one that has a very small corner prep. Check your runout before you cut. If you have to keep reseating the tool in the holder until you get acceptable runout just keep at it until you can get your runout down to .0002"-.0003" or less. This will pay off for you.

 

Mitsubishi, OSG, NS tool, and many others make fine tools that I am sure are capable, but this is the tool I have had the most success with so that is why I recommend it.

 

HTH

[Bob W.]

I am well into the job and things are going very well. I ended up using a .5" 6 flute high helix cutter recommended by my local tool supplier Western Tool and it is working great. I am using a shrink fit tool holder and a two tool strategy outlined by MotorCityMinion. Thanks for all the help.

 

Bob