High Feed Milling Cutters

[GREG]

Hello all

Can the geometry for this type of insert endmill

be input some how.

If yes will Mastercam use the geometry when processing toolpaths.

Tried a few options with facemill but its not happening for me.

 

Cheers

[2 flute]

Greg,

You want more control that what you can do here?

 

[jbel]

Greg,

 

We use Seco high feed mills and they are awesome. We take 0.04" DOC, 2" radial DOC at 750 RPM and 75 IPM in 45Rc H-13 all day long in an interrupted cut with a 2.5" face mill. This can be pushed to 150 IPM if the cut is not interrupted.

 

I define the tools as bull mills. In the manufacturer literature they give a corner radius to enter. For ours it is 0.091". This is not the actual radius but it works for defining the tool. We use these tools for roughing operations so the little bit of extra material that is left by the funky radius value that you enter isn't critical.

 

If anyone out there has never tried these mills, DO IT. If you need to remove a lot of material and you have a rigid setup, these things fly. The first time you see one run it WILL scare you but man do they work well.

[Tim Johnson]

Greg,

 

Have you tried drawing this as a custom file or custom level?

 

you can define just about any shape with this option.

 

Hint: If you do decide to draw this it would be better drawn as a custom file. This way you only have to draw it once. I keep my customs in a special tools directory.

[MIL-TFP-41]

^^^^^ Agreed

 

We have tried the Mitsubishi version on a horizontal mill. Taking a .070 DOC, at 450 RPM at 150 IPM in 440C stainless, 3" Dia cutter. I have never seen chips come out of a tool steel like that...almost like a aluminium roost. Chip load wound up being something like .075 per flute. Amazing to think that you are moving .375 per revolution. Lots of horsepower is necessary.

 

As far as defining the tool...I pretty much do the same, that is call it a bullnose endmill with a .118 radius.

[jbel]

James,

 

Seco claims that you can go up as high as .120 ipt both my ba!!s are not that brassy!!!

[robk]

I still keep on working with the Feed Mill from Iscar. At one point we had the FPT up to .110. It worked great, a little scary but great. We found it to be very comfortable @ the numbers below... BTW cutting 420SS.

 

 

[chip]

That's funny you guys should talk about this today.......Yesterday we were roughing out a piece of 17-4 ss. We were using a 1.00 R.P.F. (kennametal). A rep from Mitsubishi hands us a cutter and says here is a 1.00 (similar cutter, able to use 4 sides of the inserts by inverting the two). After we rough down the 2 parts that are behind schedule. We find out the rep gave us 1.046 inserts and scrapped our cavities.

[jbel]

Send him a bill!!!!!!