[ColletandBit]

Tried out a complex part in 6061 the other day. Wanted to share the results and feeds/speeds used and compare to what others have had success with.



I used an o-flute 1/8" bit and i have the PRO4896 and PAP Spindle from CNCRP.

16500 RPM
25 IPM
.05" DOC
WD40 as lube

Judging from some of the videos from CNCRP and ToolsToday, the feed i used is pretty conservative and i did manage to break 2 endmills...

I think the breakage was caused more by chip interference than the speeds. I had a difficult time removing chips from the cuts and i could hear grinding when the endmill reached the outer walls of the hexagon pockets...


Does anyone else cut much aluminum? If so, what have you found to be the safest speeds?

[louieatienza]

Check out my sticky in the main section... have some videos and parameters there....

[ger21]

I think your depth of cut is too deep.

[louieatienza]

I think your depth of cut is too deep.

Not necessarily if using high speed toolpaths, where a larger axial DoC is used with a smaller radial DoC to engage more of the side flutes rather than bottom, which is less efficient at cutting...

[ColletandBit]

Check out my sticky in the main section... have some videos and parameters there....

wow, i need to back out of the CNCRP forum more often, completely missed all of that stuff. Thanks!

[beltramidave]

Check out my sticky in the main section... have some videos and parameters there....

Can you post a link to your sticky? Thanks

[louieatienza]

Can you post a link to your sticky? Thanks

http://www.cnczone.com/forums/diy-cn...s-uses-22.html

[NIC 77]

I've never actually tried to mill aluminum with a 1/8" bit. Oh wait, I have. Yes, I broke the bit. Then I stuck with 1/4" minimum after that, although I have used 1/8" drill bits to peck drill holes with no problems.

1/8" bits are easy to break. Especially if they're carbide.

[louieatienza]

I actually made sort of a similar part, with a 1/8" endmill cleaning up after a 1/4" endmill... with no problems or broken bits:

Attachment 364106
Attachment 364108

The chipload may be a tad high, I try to stay around .0012-.0013" nowadays, you're around .0015". I'd keep the spindle around 12krpm and 14ipm per flute. If you climb cut, it will push the chips away from the cut. I try to stay no more than .5D DoC for picketing and .25D DoC for profiling. This is because when you profile, you have full (180deg.) engagement. Also, it helps to rough the part with a 1/4" "o" flute and leave .032" skin, then come back with the 1/8" "o" flute and do the finish pass, cutting the skin off and parting the work...

[Kosh]

Not necessarily if using high speed toolpaths, where a larger axial DoC is used with a smaller radial DoC to engage more of the side flutes rather than bottom, which is less efficient at cutting...

I'm not sure I can do that with F360. I seem to only be able to control DOC and stepover (not the same as RDOC?). So given that, what wold be a good DOC for 1/8" o-flute? I need to cut my first aluminum part soon.....

[louieatienza]

I'm not sure I can do that with F360. I seem to only be able to control DOC and stepover (not the same as RDOC?). So given that, what wold be a good DOC for 1/8" o-flute? I need to cut my first aluminum part soon.....

Axial depth of cut is the depth in Z. Radial depth of cut is the stepover... Just posted the other info below...

[Kosh]

Axial depth of cut is the depth in Z. Radial depth of cut is the stepover... Just posted the other info below...

Right, but my concern is that if you control RDOC as stepover, you still have that first pass where it is cutting full width? Will .050" be too deep for that?

either way, I just order a 1/4" o-flute and I'll cut most of it with that, then do REST processing with the 1/8" bit.

[louieatienza]

Right, but my concern is that if you control RDOC as stepover, you still have that first pass where it is cutting full width? Will .050" be too deep for that?

either way, I just order a 1/4" o-flute and I'll cut most of it with that, then do REST processing with the 1/8" bit.

You should be able to helix in which should avoid that condition...

[FoxCNC1]

I cut Alu. with a 18/" 2F. at 20 IPM with a .03-.05 DOC. I am using an off the shelf Bosch router at 8K rpm.
That is a chipload of 0.00125" My machine was not completely trammed at the time but I did get pretty good results.

I am guessing that if I could spin at 24K I could run at 60ipm or so. I am really no sure that the CNCRP PRO can run any faster or deeper in T6 Alum. I have not been able to without breaking bits.

[FoxCNC1]

I actually made sort of a similar part, with a 1/8" endmill cleaning up after a 1/4" endmill... with no problems or broken bits:

Attachment 364106
Attachment 364108

The chipload may be a tad high, I try to stay around .0012-.0013" nowadays, you're around .0015". I'd keep the spindle around 12krpm and 14ipm per flute. If you climb cut, it will push the chips away from the cut. I try to stay no more than .5D DoC for picketing and .25D DoC for profiling. This is because when you profile, you have full (180deg.) engagement. Also, it helps to rough the part with a 1/4" "o" flute and leave .032" skin, then come back with the 1/8" "o" flute and do the finish pass, cutting the skin off and parting the work...

I'd keep the spindle around 12krpm and 14ipm per flute.

Where / how did you arrive at that rule of thumb..?

I start at the chip load and go from there. Maybe do a few test cuts to see the chip size and adjust feed and rpms.
typically I cut Alum at 8K so that number along with the number of flutes are fixed. - I could be way wrong but that is how I do it.

[FoxCNC1]

To the OP. I also think you are cutting to deep for the CNCRPRO. Try 0.04 - 0.03 you can then probably try to move a little faster too.

[louieatienza]

Where / how did you arrive at that rule of thumb..?

I start at the chip load and go from there. Maybe do a few test cuts to see the chip size and adjust feed and rpms.
typically I cut Alum at 8K so that number along with the number of flutes are fixed. - I could be way wrong but that is how I do it.

It's derived from the chipload I use. Divide 14 by 12000 and it's ablout .0012". So yes, the more flutes, the faster you can go.

With a 1/8" 2-flute aluminum cutting endmill, that's 28ipm. And it scales too, so with a 2-flute 1/16" endmill I run at 14ipm and .032" DoC pocketing, .016" profiling. For 1/4, 2-flute, approximately 56ipm, at .125" DoC pocketing and .063" profiling.

There is a limit as to how fast you can go, because of the mfr. SFM ratings....

[louieatienza]

To the OP. I also think you are cutting to deep for the CNCRPRO. Try 0.04 - 0.03 you can then probably try to move a little faster too.

With the high speed, constant engagement toolpaths, you want the deepest you can go, even if that means reducing the stepover. Was doing it on my wood-framed machine almost 6-7 years ago.

[ColletandBit]

Christian Knull has some great videos focused on cutting aluminum. He has great results using trochoidal machining:

https://www.youtube.com/watch?v=p_3DK5sJgLI&t=2s

[Kosh]

Christian Knull has some great videos focused on cutting aluminum. He has great results using trochoidal machining:

https://www.youtube.com/watch?v=p_3DK5sJgLI&t=2s

Ah, ok, so Fusion360's answer to this is their "adaptive" CAM ops. So I guess that's where you do the deeper (full depth?) thing with smaller stepovers like Louie was saying.

https://forums.autodesk.com/t5/compu...g/td-p/5860958

But playing with it, I can't get the helix entry to work (the setting is there, but it's still plunging).