[4]

Recommendation for face mill

[3]
[10] Like what you see?
Click here to donate to this forum and upgrade your account!

PT Doc

Active User
Registered
Joined
Dec 27, 2012
Messages
274
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:

mksj

Active User
H-M Supporter - Gold Member ($25)
Joined
Jun 12, 2014
Messages
2,094
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.
 

PT Doc

Active User
Registered
Joined
Dec 27, 2012
Messages
274
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
 

Mitch Alsup

Active Member
Registered
Joined
Nov 17, 2017
Messages
401
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?
 

PT Doc

Active User
Registered
Joined
Dec 27, 2012
Messages
274
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.
 

PT Doc

Active User
Registered
Joined
Dec 27, 2012
Messages
274
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
 

PT Doc

Active User
Registered
Joined
Dec 27, 2012
Messages
274
Using the carbide depot link:
4” cutter diameter, all 6 inserts, 4” WOC, 350 SPM

653D3352-A40A-48CD-A250-A6D5E3EA5B42.jpeg
 

PT Doc

Active User
Registered
Joined
Dec 27, 2012
Messages
274
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
 

PT Doc

Active User
Registered
Joined
Dec 27, 2012
Messages
274
Using the carbide depot link:
5” cutter diameter, all 8 inserts, 5” WOC, 350 SPM

4C63147C-1396-468A-88D8-D2CD37113E0A.jpeg
 

PT Doc

Active User
Registered
Joined
Dec 27, 2012
Messages
274
Using the carbide depot link:
5” cutter diameter, all 8 inserts, 4” WOC, 350 SPM

027DA315-B50F-4BD9-B6DC-6D634455AB92.jpeg
 

Shootymacshootface

Active Member
Registered
Joined
Mar 17, 2018
Messages
323
First, I am the farthest thing from a feeds and speeds guru.
I have a 3hp knee mill, and the first face mill I bought was a 3" which works great on almost everything. I noticed that I was using it on a lot of smaller parts and it doesn't run smoothly unless you have several cutters engaged on the work at the same time. I just got a 2" face mill, but haven't used it yet.
I don't think you will have a power issue with a 5hp mill.
 

PT Doc

Active User
Registered
Joined
Dec 27, 2012
Messages
274
Using the carbide depot link, the number for cubic inches removed are as follows:
Also going on G Morsch’s conversion of 1 cubic inch removal =~1hp.

4” cutter diameter, all 6 inserts, 4” WOC, 350 SPM. -=>4.5 cubic inches. ~4.5hp.

5” cutter diameter, every other insert installed for total of 4 inserts, 5” WOC, 350 SPM. -=>3.0 cubic inches. ~3.0hp

5” cutter diameter, all 8 inserts, 5” WOC, 350 SPM. -=>6.0 cubic inches. ~6hp :(

5” cutter diameter, all 8 inserts, 4” WOC, 350 SPM. -=>4.8 cubic inches. ~4.8hp

So many numbers, still a bunch of questions. Are interrupted cuts with a face mill less than ideal? For less wide material, a 1” or 1.25” indexable end mill seems like it would be better.
 

mksj

Active User
H-M Supporter - Gold Member ($25)
Joined
Jun 12, 2014
Messages
2,094
The positive rake requires less Hp (FM45) I use a 2.5" in aluminum with no issues and also have a 4" with 7 inserts, I use a 2" for ssteel with an R8 and 3 Hp motor. The calculations or for maximum material removal which is seldom the case as a hobbyist. I would not leave out inserts as it will effect the surface finish. As mentioned I would probably go with a 4" FM45 for softer materials and a a 3 or 4" FM90 for harder materials and shouldering with a heavier mill and 5 Hp. You could get a single arbor. I like the larger head for wider stock, but can also be used on smaller stock. You need accurate head alignment, I get almost mirror surface. I use some air to clear the chips.
 

PT Doc

Active User
Registered
Joined
Dec 27, 2012
Messages
274
The positive rake requires less Hp (FM45) I use a 2.5" in aluminum with no issues and also have a 4" with 7 inserts, I use a 2" for ssteel with an R8 and 3 Hp motor. The calculations or for maximum material removal which is seldom the case as a hobbyist. I would not leave out inserts as it will effect the surface finish. As mentioned I would probably go with a 4" FM45 for softer materials and a a 3 or 4" FM90 for harder materials and shouldering with a heavier mill and 5 Hp. You could get a single arbor. I like the larger head for wider stock, but can also be used on smaller stock. You need accurate head alignment, I get almost mirror surface. I use some air to clear the chips.
Are interupted cuts an issue for insert durability and surface finish?
 

mmcmdl

H-M Supporter - Gold Member
Staff member
H-M Supporter - Gold Member ($25)
Joined
Jan 31, 2016
Messages
1,441
Are interupted cuts an issue for insert durability and surface finish?
Not at all . It's an insert cutter and always has interrupted cuts ! Not sure how it would have a continuous cut ? :confused 3:
 

PT Doc

Active User
Registered
Joined
Dec 27, 2012
Messages
274
Not at all . It's an insert cutter and always has interrupted cuts ! Not sure how it would have a continuous cut ? :confused 3:
I didn’t phrase it properly. With a 4” diameter face mill on 2” wide stock, the inserts will engaging the material and then coming off of the part. With a 1.25” indexable end mill on 2” stock, the end mill and inserts would not be coming off the part the same. No?
 

mmcmdl

H-M Supporter - Gold Member
Staff member
H-M Supporter - Gold Member ($25)
Joined
Jan 31, 2016
Messages
1,441
Wouldn't make a difference . An insert on a mill cutter is never fully engaged in a cutting action . It cuts in then 180 degrees it's out . Make sense ? The cutter is still parallel with the bottom cut but not actually cutting .

By the way , I'm an old time Kennemetal and Valenite guy . :encourage:

I understand what you're saying though ! You're talking about re-entering the workpiece with a larger cutter . With the correct grade carbide this has little to no effect . I believe Valenite V02s were the insert of choice years ago .

I may add , why would anyone use an undersize facemill other lack of HP ? Just adds time to the job ! :)
 
Last edited:

PT Doc

Active User
Registered
Joined
Dec 27, 2012
Messages
274
Wouldn't make a difference . An insert on a mill cutter is never fully engaged in a cutting action . It cuts in then 180 degrees it's out . Make sense ? The cutter is still parallel with the bottom cut but not actually cutting .

By the way , I'm an old time Kennemetal and Valenite guy . :encourage:

I understand what you're saying though ! You're talking about re-entering the workpiece with a larger cutter . With the correct grade carbide this has little to no effect . I believe Valenite V02s were the insert of choice years ago .

I may add , why would anyone use an undersize facemill other lack of HP ? Just adds time to the job ! :)
Thank you. Sounds like the the 4” would be a good choice for my 40 taper 5hp machine? Since I will only be getting one face mill initially, do you think the 45* SEHT..... style is the most versatile?

https://www.glacern.com/fm45

E171D91A-C195-43B3-9546-390E80520A71.png

07A46680-D296-4E85-AEEF-E5F39B3CB655.png
 

mksj

Active User
H-M Supporter - Gold Member ($25)
Joined
Jun 12, 2014
Messages
2,094
Yes, a 4" FM45 would be good for facing, but not shouldering. If shouldering I would probably go with a 3" FM90. There are various inserts available and coatings, some can be used on a wide range of materials.
 
[6]
[5] [7]
Top