What's new
What's new

Who Makes the Absolute Best Roughing Endmill for Aluminum?

I vote for Hanita TC6A0R13005. 1/2" x 1.25" LOC. If you need smaller diameter, they don't offer this series smaller. On a standard 10k rpm Speedio, I have removed 103 cubic inches per minute of 6061. Cutting parameters were 10k rpm, 1.25" Axial loc, .300" radial stepover at 275 IPM. Has Weldon flat, hold with side lock end mill holder. Day in and day out on a 16k or 27k spindle machine, I would run about 1" Axial, .250" stepover and 250 IPM ish.
I looked at the suggested feeds and speeds on this and several of the other recommended tools. Recommended depth of cut for this stepover and feed is half what you were doing. Did you get there by just cranking up feed and or stepover until you broke a tool?
I looked up my typical metal removal and it is 1/4 the above. I will have to see which of the above roughers my local dealer can get. They don't list any of these companies on their website but I suspect they carry some of them.
 
Best part of needing draft on everything, shank on long tools don't rub. :D
My molds are small and I have a bad habit of buying 1/8" shank tools, so even with draft the tools need to be relieved. But that's a self inflicted problem.

Back on topic- are these Accupro roughing and finishing end mills the same as Alumigators? They look identical, not sure if they're a copy or private label from GWS. Either way they work well, and used to be under $30 to boot (for those of us that don't hate money).

 
My molds are small and I have a bad habit of buying 1/8" shank tools, so even with draft the tools need to be relieved. But that's a self inflicted problem.

Back on topic- are these Accupro roughing and finishing end mills the same as Alumigators? They look identical, not sure if they're a copy or private label from GWS. Either way they work well, and used to be under $30 to boot (for those of us that don't hate money).

Not sure, the picture does look very similar, though I don't trust stock photos on msc for anything. Looks like they are $50 a piece which is the same price as the GWS tool so you're not saving anything.
 
Garant Hoffman master Alu line has done really well for me. Specifically slot machine HPC. These are DLC coated corn cob cutters with through coolant. You can run pretty much any strategy on it. Vertical plunge, slotting , steep ramp and 1/2D traditional tool paths, 10% to 50% engagement dynamic tool paths… Ceratizit, Emuge, Hoffman Vratny all have similar offerings with similar capabilities should be able tom find imperial sizes somewhere. I've run many many brands of aluminum end mills and have settled on these. They’re in the same price range as the kor5 and a good cunk less than OSG aero-o-ETS.

 
I looked at the suggested feeds and speeds on this and several of the other recommended tools. Recommended depth of cut for this stepover and feed is half what you were doing. Did you get there by just cranking up feed and or stepover until you broke a tool?
I looked up my typical metal removal and it is 1/4 the above. I will have to see which of the above roughers my local dealer can get. They don't list any of these companies on their website but I suspect they carry some of them.
Wildman Rob at MasterCam was showing off Dynamic milling back in the day. He said we are going to pocket that out at full depth of cut and .300" stepover at 200 IPM. I said no way! He said "go for it" and the rest is history. Since then I have pushed that to 275 IPM before bogging the spindle. Haven't pushed it on a High Torque yet.
 
Wildman Rob at MasterCam was showing off Dynamic milling back in the day. He said we are going to pocket that out at full depth of cut and .300" stepover at 200 IPM. I said no way! He said "go for it" and the rest is history. Since then I have pushed that to 275 IPM before bogging the spindle. Haven't pushed it on a High Torque yet.
What happens when you "bog" the spindle? It would be nice to learn from others on this as I figure it out. I will be testing this soon with a 13/16" drill at lower speeds in 6061.
 
I decided from reading this thread, and while reviewing other peoples programs that were painfully slow, leaving money on the table, I decided to try a Destiny Diamondback. I went after it, 6061-T6, 1/2 mill, 10,000 RPM, 3/4 deep, 225 IPM with a .150 step over ramping into the pocket, and I could have easily pushed it more, only problem was I had to back it off as warping was becoming an issue. I backed it off to 160 IPM and the part is staying flat.
 
What happens when you "bog" the spindle? It would be nice to learn from others on this as I figure it out. I will be testing this soon with a 13/16" drill at lower speeds in 6061.
Bogging is when you can actually hear the spindle slowing down. 13/16 drill in good 6061 shouldn't be a problem on a 16k depending on the cutter. Watch your spindle load. Adjust feed to keep load just under red and the machine should be happy.
 
very impressive stuff!

i'd be very curious what that thing would do with a fraisa AX-FPS rougher, would you be interested in doing a test? i can get my rep to send you a tool for free
A bit late but here is the update. Eugene (empower) came to our showroom and we ran the Fraisa 12mm rougher on a standard 16k spindle S series speedio, standard BT30 non-dual contact end mill holder. 1.25" Axial doc, .300" Radial doc, 275 IPM. Roughed out the test piece in about 15 seconds.
 

Attachments

  • 20220822_121709_resized.jpg
    20220822_121709_resized.jpg
    243.7 KB · Views: 48
  • 20220822_121909_resized.jpg
    20220822_121909_resized.jpg
    278.4 KB · Views: 48
  • 20220822_121915_resized.jpg
    20220822_121915_resized.jpg
    221.2 KB · Views: 49
  • 20220822_121927_resized.jpg
    20220822_121927_resized.jpg
    413 KB · Views: 48
A bit late but here is the update. Eugene (empower) came to our showroom and we ran the Fraisa 12mm rougher on a standard 16k spindle S series speedio, standard BT30 non-dual contact end mill holder. 1.25" Axial doc, .300" Radial doc, 275 IPM. Roughed out the test piece in about 15 seconds.
that was pretty fucking impressive! one day i'll have one of your machines :)
 
International Minicut, hands down. They annihilate aluminum, I've never had flutes get clogged, the hi speed steel is more forgiving then carbide. Good tool life, make sure they have adequate coolant, the few I have broken have just snapped, no shards of carbide to dig out of your part . I ve also had good luck with the square tooth Fettee ruffers.
 
That Fraisa looks impressive! That's a 100 cubic inch cut

For quite a bit less money (but still expensive) I like the Hoffmann slotmaker. The manufacturer claims you can ramp up to 45 degrees (?!). They come in long length or shorter length with CTS.

Here's a 75 cubic inch cut with a fairly long gauge shrink holder. There video actually shows a 12mm Garr because I broke the Hoffmann just before I wanted to film the cut...🙈 The Garr needed the ramp turned right down and tons more coolant (the Hoffmann i had the flood off).

Spindle load was about 5 blips (middle of the green). Less with the Hoffmann. I was nervous to push it, but couldn't see a reason not to...

I went smaller stepover and higher chipload than your cut. Not sure if that's the best way to run these?

 
That Fraisa looks impressive! That's a 100 cubic inch cut

For quite a bit less money (but still expensive) I like the Hoffmann slotmaker. The manufacturer claims you can ramp up to 45 degrees (?!). They come in long length or shorter length with CTS.

Here's a 75 cubic inch cut with a fairly long gauge shrink holder. There video actually shows a 12mm Garr because I broke the Hoffmann just before I wanted to film the cut...🙈 The Garr needed the ramp turned right down and tons more coolant (the Hoffmann i had the flood off).

Spindle load was about 5 blips (middle of the green). Less with the Hoffmann. I was nervous to push it, but couldn't see a reason not to...

I went smaller stepover and higher chipload than your cut. Not sure if that's the best way to run these?

i've gotten over 200 cubes with the fraisa 20mm rougher and pretty sure i could push it to 300+ next time i play with it
 
i've gotten over 200 cubes with the fraisa 20mm rougher and pretty sure i could push it to 300+ next time i play with it

Oh my word! That's insane! Tell us more!!

Question: Why do we need a 20mm to do something like that? Seems like a 12mm tool should be sufficiently strong enough to get into the 100-150 cubes range. And assuming you can do that cut on a 16k spindle, then by definition the tool forces must be lower than my tool calculator is predicting, so perhaps more cubes are possible? Might seem like a 16mm would have plenty of strength to play in this game?

Any tips for how to rough on a little (dual contact) Speedio? If we assume 100 cubes, then is it easier on the machine to run more step-over? More depth of cut? More chipload? What's the best way to design a cut for machine safety, if targetting a certain removal rate?

Perhaps naively I've tended to go with max length of cut, shallow step over (20% seems about peak for chip thinning benefits) and then increase the chipload until I'm scared? However, I'm not really sure what the clues are that I'm going to break something expensive? Length of cut seems to increase tool pull down forces, plus increasing sideways forces on the taper interface. Increasing step over or feed seems to affect spindle torque and sideways forces. How best to balance all these things?
 
Oh my word! That's insane! Tell us more!!

Question: Why do we need a 20mm to do something like that? Seems like a 12mm tool should be sufficiently strong enough to get into the 100-150 cubes range. And assuming you can do that cut on a 16k spindle, then by definition the tool forces must be lower than my tool calculator is predicting, so perhaps more cubes are possible? Might seem like a 16mm would have plenty of strength to play in this game?

Any tips for how to rough on a little (dual contact) Speedio? If we assume 100 cubes, then is it easier on the machine to run more step-over? More depth of cut? More chipload? What's the best way to design a cut for machine safety, if targetting a certain removal rate?

Perhaps naively I've tended to go with max length of cut, shallow step over (20% seems about peak for chip thinning benefits) and then increase the chipload until I'm scared? However, I'm not really sure what the clues are that I'm going to break something expensive? Length of cut seems to increase tool pull down forces, plus increasing sideways forces on the taper interface. Increasing step over or feed seems to affect spindle torque and sideways forces. How best to balance all these things?
not on a speedio of course... that was done on a zimmerman 5 axis gantry with a 50hp spindle. doubt a speedio would be able to do much more over 100 cubes but i've been proven wrong before...
i have no personal experience running speedios so i'll let someone else chime in on that.
i would imagine higher chip load would be better on a machine like that.
 
Any tips for how to rough on a little (dual contact) Speedio?
We had a repeat job making thousands of aluminum boxes on our Speedio.
I was running a 1/2" Destiny Diamondback 3 flute,16k rpm, 400+ipm, 20% stepover, 1.28 deep. That tool lasted anywhere from 6,000 parts to 10,000 parts pocketing 4"x4" stock out to a .06" wall thickness 1.28 deep.
 








 
Back
Top