Recommendation for face mill

PT Doc

Active User
Registered
Joined
Dec 27, 2012
Messages
348
What would be an appropriate diameter facemill for a 5hp manual knee mill? Milling machine will be modified to accept CAT40 tooling? Material milled will be hardened and non hardened steel and aluminum. Maybe occasionally some delrin

Quill diameter is 4 1/8” and max rpm is 3800.

Thank you for your recommendations.
 
Last edited:
I would also look at Glacern in a 4-5" head, typically raked FM45 for aluminum, FM90 for steel.
https://www.glacern.com/fm45
https://www.glacern.com/fm90

I have picked up heads from Iscar, Sandvik and Kennametal. They work well but expensive if purchased new. Also some have proprietary inserts, so you need to check availability and pricing. I would recommend something like the Glacern or Maritool.
 
I would also look at Glacern in a 4-5" head, typically raked FM45 for aluminum, FM90 for steel.
https://www.glacern.com/fm45
https://www.glacern.com/fm90

I have picked up heads from Iscar, Sandvik and Kennametal. They work well but expensive if purchased new. Also some have proprietary inserts, so you need to check availability and pricing. I would recommend something like the Glacern or Maritool.

Thank you from rather response. In your opinion, if I was getting face mill, should I get a 45 or 90*? Sounds like either might be a compromise to use on all materials but if 45* is ideal on aluminum and 90* on steel, is 45* better on steel than 90* is on aluminum? Maybe not worded super cleanly but which is the least lousy on the nonideal material? Thanks again
 
What would be an appropriate diameter facemill for a 5hp manual knee mill? Milling machine will be modified to accept CAT40 tooling? Material milled will be hardened and non hardened steel and aluminum. Maybe occasionally some delrin

Quill diameter is 4 1/8” and max rpm is 3800.

When using a face mill it is generally the lowest speed possible that determines how big a face mill one can use. So, what is the min RPM?
 
When using a face mill it is generally the lowest speed possible that determines how big a face mill one can use. So, what is the min RPM?

Min RPM is 80 for this machine.

Seems like a face mill with an even number of inserts could be more versatile since I could remove every other insert.
 
G Morsch Carbide guy responded in another thread to me when I inquired about an R8 facemill.

https://www.hobby-machinist.com/threads/facemill-options.70339/#post-589327

Insert milling cutters are great! And your choice is particularly good for most materials. I was a technical resource for Kennametal salesmen for 35 years and milling was always fun. The 20 deg. positive insert with the "H" tolerance is tough to beat. Now, the R8 platform is very good for small diameter milling cutters, but, they do have some limitations. I would recommend the 2.5" cutter with 5 inserts, but if you need the 3"diameter and plan to take a full width cut, you may want to remove 3 of the inserts so you don't run out of horsepower and stall the spindle. Bad news on a knee mill since the feed motor may continue to drive the table.
There is a simple metal removal calculation that will work for just about any application you will ever encounter. Only materials that are very high strength will need reduced parameters. Most metals, including pre-heat treated 4140, 17-4PH, 15-5PH, stainless steel, and many others will machine at 1 cubic inch per minute, per horsepower. To calculate a cube we only need three dimensions, length in per minute IPM), depth of cut (DOC), and width of cut (WOC). To calculate hp. requirements multiply IPM x WOC x DOC.
Example:
A 2.5" cutter has a periphery of .6545 ft. A 2" Width of cut on 4140 bar stock would run easily at 350SFM, 535RPM. With a feed per tooth of .005, the IPM would be 13.375" (5 x .005 x 535). A 2" WOC would allow 3 hp. to be consumed at a depth of cut of .112DOC.
13.375 IPM x 2" WOC x .112 DOC = 3 cubic inches per minute and at 80% efficiency, that equals roughly 3 hp. and gives you a little wiggle room for positive vs. negative, dull vs. sharp, etc.
For a couple of other materials:
Aluminum will net 2 to 4 cubic inches per minute
Cast Iron will net 2 cubic inches per minute (G3000, G3500, G4000 CI)
TiAlN/ALTiN coatings are universal and work well on many materials. Since your knee mill has fairly limited rpm compared to CNC machines, choose tough grades for best durability. Grades described as 30, 35, 40 will give excellent service and they will take a beating. Higher the number, the tougher the grade, but you will sacrifice a little wear resistance and a little heat resistance. For Aluminum go uncoated, TiCN, or TiB2 for best results.

Good luck with the new cutters.
Best Regards, Gary
 
Using the carbide depot link:
4” cutter diameter, all 6 inserts, 4” WOC, 350 SPM

653D3352-A40A-48CD-A250-A6D5E3EA5B42.jpeg
 
Using the carbide depot link:
5” cutter diameter, every other insert for total of 4 inserts, 5” WOC, 350 SPM

CF488D67-2ABE-4FD8-A980-F0C75FA44C1B.jpeg
 
Back
Top