Long Length Endmills

[Miller846]

Hi, I am curious what all of your thoughts are on this. I need to machine about 80 aluminum blocks, roughly 3.5” x 4” X 5”. My plan is to just face the top and drive around the sides with a 1” Diameter Long Length endmill. But I am concerned about chatter doing something like this. Has anyone ever used a reduced shank endmill and taken step downs for profiling thicker stock? I’m curious if it would leave lines at each step down or if it would leave a better surface finish than a long length. Unfortunately, I currently only have a 3 axis mill, otherwise I would just face mill each side. Let me know your thoughts, thanks!

 

[Mechanola]

I hate endmills. And aluminium

Flip the parts in a smart fixture and use a large facing head.

 

[Orange Vise]

Relieved shank endmills will leave lines but give you better perpendicularity.

Long length endmills will give you a taper but a better finish.

 

[Greg White]

Or get a 1"enmil ground with back taper for a .002 pass.
Gw

 

[Milling man]

Relieved shank endmills will leave lines but give you better perpendicularity.

Long length endmills will give you a taper but a better finish.

 

[Milland]

With a decent CNC mill and setup, and especially with a 1" carbide endmill on aluminum, sometimes just a spring pass or two will get you a good perpendicular cut. But finding the "sweet spot" for S/F for the finish pass can take some experimenting.

I usually vary the height a bit, perhaps .010" high on the first spring, then final depth on the second.

 

[MCritchley]

I use relived shank cutters from Helical tools for stepping down the perimeter on Al parts often. I’ll hold the work piece with some Talon grip jaws, face the top and step mill the sides. That process leaves me with five milled sides that are within a thou of perpendicular and parallel. I always have a 3” reach endmill mounted so I can mill a 2.8” tall part. The steps are there, but you can hardly detect them with an indicator of profilometer. And while I’m at it I’ll chamfer in the machine so I don’t need to debur by hand.
I’ll mill off the waste on opp 2. and chamfer that side also.

Stepping down is a very efficient and controlled way to mill a part. Full length endmills are not as stiff as a relived shank tool and as others have said will leave a tapered wall.

 

[cmccull166]

IMCO is advertising a endmill for deep pockets.
I have no experiance using one.

 

[DavidScott]

The end mill matters. A 7+ flute will work much better than a 3 flute since it has soooo much more core strength. I say a full length cut is doable, depending on what is holding it.

 

[crossthread82]

I wouldn't be attempting that in one cut unless you're using a 5+ flute endmill, something like the AF5 from Swiftcarb. 3 flute at that L to D ratio is starting to get flimsy. I ramp contour with necked endmills all the time. Is it going to leave a mirror, no. But the step downs are very minimal and you can't feel them at all, just kind of looks like a light shadow on the wall. With an endmill over 4xD you'll need a spring pass to bring in the perpendicularity. With a necked tool its likely not necessary.

The key with a necked tool is to ramp down the wall instead of depth cuts. That keeps the tool in contact with the wall at all times, making it more seamless.

 

[DSMWerks]

YG-1 Alu-Power extended reach/necked will blow your mind how seamless it can be. I rough it leaving .002" then Helical ramp around the profile until it reaches the bottom. Never seen a sharper end mill.

 

[50BMG DUDE]

YG-1 Alu-Power extended reach/necked will blow your mind how seamless it can be. I rough it leaving .002" then Helical ramp around the profile until it reaches the bottom. Never seen a sharper end mill.

I'll second this - This is my goto for tall parts as well.

 

[OVodov]

If looking for perpendicularity you will need not only tool but holder too.
Shrink fit or hydraulic would be the best.
For rough I would say to use long chipbraker.
For finish take the tool with 5 flutes.
Kennametal KOR or similar Helical or Imco. I love Imco

 

[OVodov]

I have used OSG 4 flutes for long reach finishing in precision bore and got perpendicularity to face within 0.0012 along 3”.
So use as many flutes as you can find, it gives better flatness, but keep it in mind to hold it perfectly.
And use it only for finish, Endmills with many flutes don’t have room for chips.

 

[MCritchley]

YG-1 Alu-Power extended reach/necked will blow your mind how seamless it can be. I rough it leaving .002" then Helical ramp around the profile until it reaches the bottom. Never seen a sharper end mill.

What is your typical ramp angle with a .002” cut?

 

[13engines]

What is your typical ramp angle with a .002” cut?

I can't answer for D smith, but common sense would say your -Z move would be just shy of one full flute length per time around the part. That is if the part periphery was long enough. At 0.002 of material to remove, I doubt there is any angle sharp enough to be bad for the cutter like it might be for ramping or helical milling into solid, but there could be an angle too sharp to give a usable finish. Perhaps D smith has the answers for that. I haven't tried this yet, but it isn't a bad idea compared to running a very long end mill.

After further thought, how do you get past the double cutting that will have to occur at the beginning and ending of the tool path? Is it cut one flute length and then a quick ramp to the next level? This would make your transition areas move around the periphery of the part as you progress down each level. Hopefully D smith can explain.Or anyone for that matter.

 

[50BMG DUDE]

I always use a constant Z toolpath for profiling, about 0.1-0.200 depth per pass dependent on the cutter size

 

[couch]

roughly 3.5” x 4” X 5”

How deep do you actually need to cut?

Have had real good results with solid carbide endmills in hydraulic holders going around 4” deep. Under a thou total taper side to side in aluminum with nice finish, no chatter. Rougher in an ER32 (no reason other than I have a bunch) than finisher in the Hydraulic. Would easily go deeper especially if I bumped it to 1” diameter. Slow rpm (around 2500rpm), slow feed and clear chips before the finish pass either manually or with good coolant flow or air blast with coolant. Also ran a spring pass.

Unfortunately can’t show the parts with any detail, may be able to take some photos of one of the setup pieces that I still have though to show the sidewall finish if interested.

Long story short, run a long tool, dial in the runout and don’t try to spin it too fast. Will work fine, it’s aluminum.

 

[DSMWerks]

When I use Z ramp profile to finish pass with YG-1 Alu-Power I go about 3/8"-1/2" ramp per pass. I don't use the same end mill as I roughed with so the finish end mill is razor sharp. On a 3/4" Alu-Power Extended reach the cut length is 1" and the solid shank does a great job of not flexing. To me its all about the razor sharp edge. You can have 6-7 flutes but if the 3 flutes on Alu-power are twice as sharp it will do a better seamless job.

 

[crossthread82]

When I use Z ramp profile to finish pass with YG-1 Alu-Power I go about 3/8"-1/2" ramp per pass. I don't use the same end mill as I roughed with so the finish end mill is razor sharp. On a 3/4" Alu-Power Extended reach the cut length is 1" and the solid shank does a great job of not flexing. To me its all about the razor sharp edge. You can have 6-7 flutes but if the 3 flutes on Alu-power are twice as sharp it will do a better seamless job.

Flute count doesn't really matter if the tool is necked since the solid shank is supporting it. In long LOC endmills though, flute count is everything b/c that's where all your strength is coming from.