[Magnum164]

have you taken into consideration that a 4 flute may be beneficial ? the tool will have more rigidity and you'd have double the cutting edges , which will gain you twice the feed rate .
i realizes that 4 flutes on aluminum seems to have become a false taboo , but considering the light chip load on such a small tool then chip welding isn't much of an issue if there is ample coolant .
I got an aluminum production job up and running today which I needed to use a 3/16 for a lot of slotting , in order to speed up the process I threw in a 4 flute and it works great at 10000 rpm , 50 ipm , .125 depth of cut .
needs a quick finish pass but its to be expected with a small tool

I generally use nothing but 4FL. I actually started using the 2FL when I tried to to the "run from here" and lost my only 4FL...

But if you are getting that kind of speed.... Is that correct at .125 DOC? I assume that was Carbide as well?

I had started using 2FL when I started pocketing as most info I saw stated to use 2FL to avoid chip packing when slotting. But, I have since read what you have said that as long as you have good chip removal, 4FL are not an issue and can actually be better.


Just a note. I'll try some more things once I verify my machines RPM, tach should be here by Fri. I have also sent a note to Tormach to check on my VFD calibration. Seems when I had to reload my control box a while back I never went back and calibrated the spindle. The spindle steps where definitely not what was listed in the manual. I don't know that much about VFD's and how much that would have actually affected the RPM. The machine definitely has a different pitch sound now at S1000.

[dertsap]

But if you are getting that kind of speed.... Is that correct at .125 DOC? I assume that was Carbide as well?

.

yes that's a carbide with .125 depth of cut , its no fascinating speed and feed but the tool was at hand and for the time being it works for what i need it to do , I tend to have a bit of a passive aggressive approach to machining , especially if something is heading for production , i like to know that the machine can be wlaked away from and i wont come back to a carousel of broken tools . I suppose its shell shock from running large expensive parts but I tend to like to make things run as fast and safe as possible

usually for heavy slotting 2 flute is the better choice , but as i stated , the chip load is so light on a small tool that the chips tend to be small , so with a decent blast of coolant to keep the area clear then chip welding isn't a problem .

[Peter H]

Personally have had better luck with HSS on Aluminum than Carbide for small cutters. Carbide cuts beautifully but just one boo-boo and you are replacing a cutter. Takes a lot more time to replace a broken cutter than just running slower and the idea it get the part out in the quickest time. Would at least optimize a program with HSS then switch to carbide once you are happy with it.

The seat-of-the-pants method of assessing how the program is doing is by looking and listening. Look at the chip size being made at different points in the program. Bigger chips means bigger cutter load and generally can addressed by increasing RPM during those cuts. The louder the cutter is groaning, the more you are working it keeping in mind that it is relative.

Looking at how the program was running in the video much earlier in this thread, there are opportunities to speed up feed when taking lighter cuts and slow it down when taking the heavy cuts. There was a fair amount of non-cutting vertical motion that could be G00. I don't know any way to do this other than brute force going through the program and adding and changing feed rates. You may be able to do some in your CAM program by changing approach feed rates. Doing the brute force editing on a pretty complex program like you have will take an investment in time and it is soo easy to fat finger something, but is doable if you have the right personality (like to play solitaire for days on end, like to count count the number of screws that come in a box, etc.)

[Wog]

[QUOTE=Peter H;996391]There was a fair amount of non-cutting vertical motion that could be G00. I don't know any way to do this other than brute force going through the program and adding and changing feed rates. QUOTE]

I use Notepad for most of my code editing, usually right at the Tormach. "Replace All" command works great for changing to G00. I also try to use lower case "g00", "m7", etc. and then use the "Match Case" feature to find and replace items I've already changed.

[Magnum164]

@Peter/Wog

The slow plunge moves were deliberate I just forgot to set them back when I made that video....

[beco]

I've found a simple feed / speed table that is nice for quick reference.

May not be optimized much, but very useful to get into a ballpark that works


End Mill and Cutting Tool Speed and Feed Calculations

Hope this helps a little.

[DMF_TomB]

you do not mention length end mill sticking out or coolant use

1) long end mills need a reduced Depth of cut
2) coolant or oil helps prevent chips sticking to flutes which if happens can break end mills

sample parameters based on my calculations

diameter 0.125 HSS end mill 2 Flute
Stickout from collet 0.75
327 SFPM
Coolant minimal oil sprayed or brushed on
chip thickness 0.001
10000 rpm
Feed 21 ipm
DOC 0.017
Cutter tip force 0.5 lbs

Stickout from collet 1.0
chip thickness 0.0008
Feed 16 ipm
DOC 0.010
Cutter tip force 0.2 lbs

Stickout from collet 0.5"
chip thickness 0.0016
Feed 31 ipm
DOC 0.039
Cutter tip force 1.7 lbs

[Magnum164]

I've found a simple feed / speed table that is nice for quick reference.

May not be optimized much, but very useful to get into a ballpark that works


End Mill and Cutting Tool Speed and Feed Calculations

Hope this helps a little.

Thanks, will check it out.

[Magnum164]

You can see in the video that it was flood coolant, not a heavy flood, but was enough to keep the chips out.

The endmill's I broke were probably no more than .75 or .5IN out. Most of the materials I cut have been less than .25IN in thickness.


I will say that I recalibrate my Spindle. Seems you need to do that after you reload the controller software. Not sure where I was when I started, but after calibrating the machine is definitely turning higher RPMS. I am off at the higher RPMS. For instance at 1K I am probably within 10-20 RPM, 4-5K RPM I am within 75-100 and at 10K RPM I am running 120RPM higher. Not that great of number difference, but this is after calibration. No telling what I was running before it was calibrated.

you do not mention length end mill sticking out or coolant use

1) long end mills need a reduced Depth of cut
2) coolant or oil helps prevent chips sticking to flutes which if happens can break end mills

sample parameters based on my calculations

diameter 0.125 HSS end mill 2 Flute
Stickout from collet 0.75
327 SFPM
Coolant minimal oil sprayed or brushed on
chip thickness 0.001
10000 rpm
Feed 21 ipm
DOC 0.017
Cutter tip force 0.5 lbs

Stickout from collet 1.0
chip thickness 0.0008
Feed 16 ipm
DOC 0.010
Cutter tip force 0.2 lbs

Stickout from collet 0.5"
chip thickness 0.0016
Feed 31 ipm
DOC 0.039
Cutter tip force 1.7 lbs

[DMF_TomB]

length an end mill sticking out can have a big effect. 1/4" difference in length can have a big effect
.
a stub length end mill is about 1.5 to 2 diameters long so 1/8 dia would be about 3/16 to 1/4 long.
.
a regular length end mill is about 2 to 3 diameters long so 1/4 to 3/8 long
.
what most people do not realize is a stub length can usually take 2-3x the depth of cut of a regular length end mill
.
also you need to watch chips plugging or clogging in the flutes. some times compressed air blowing at the end mill can help with keeping the flutes clear of chips.
1/8 dia em HSS (less brittle and less likely to snap off from sudden movements)
3/4" sticking out
at a slow 133 SFPM
rpm 4000
Feed 8.5 ipm
DOC 0.035
load on end mill 0.4 pounds at 10% load
end mill should not have more than 4 lbs on end (it will maybe break)
at
1/2" sticking out
Feed 12.7 ipm
DOC 0.078
load on end mill 1.4 pounds at 10% load
end mill should not have more than 14 lbs on end at maximum
...... notice the shorter end mill is stronger and can take more pounds of force