How fast can I go? Safely...

[lemo]

I am routing my first relief on my TAIG. Yessssssssssss!
I use a 3/32nd carbide ball end mill with a 1/4 tool diameter step over in MDF.
Works like a charm with 4IPM at up to a maximum 0.25 Inch cutting depth.
It seems... that I can go much faster. I started with 2IPM and now I tweaked it up to 4IPM.
Sounds good, no heat, simply carving away happily.
What would be the professional recommendations?

Is there a general table/rule of thumb/formula which can yield a recommended maximum speed for cutters and materials?
Or is this where the experience and the broken cutters start?
I plan to use aluminium at one stage.... but hesitate right now as I have no experience there.
One IPM might be to fast already... No idea.... so I stay away for now.

Thanks in advance for some insights
Lemo

[Graham Waterworth]

Here are some formulas :-

D     = Diameter of cutter
T     = Number of teeth
RPM = Revs per min
F     = Feed
FT   = Feed per tooth
S     = Peripheral speed of cutter
PI    = 3.1416

Cutter speed

S (ft/min) = D*PI*RPM
                ________  = 0.2618D*RPM

                      12

S (m/min) = D*PI*RPM
                  ________
                     1000

Cutter revolutions


RPM = S (ft/min)
          ________
           0.2618D

RPM = S (m/min)*1000
         ______________
               PI*D


Feed per tooth

The suggested feeds are based on 1*dia for axial depth and 0.5 * dia for radial depth of cut.

Cutter dia             Feed per tooth

inch     mm           inch     mm

5/64    2.0           .0003   .0075
1/8      3.0           .0005   .013
1/4      6.0           .0010   .025
1/2    12.0           .0015   .037
1       25.0           .002     .050

FT =           F
             ______
             T*RPM

To increase axial depth to :-

1-1/2 *D reduce feed by approx 30%

2 * D reduce feed by approx 50%

To reduce radial depth to :-

1/4 * D increase feed by 200%

1/8 * D increase feed by 250%

Cutter feed

F = FT*T*RPM

Graham.

[lemo]

Excellent! Thanks you so much Graham.
I did a search on cutting MDF and ran into the chipload formulas.
Good stuff. Now I also understand why high rpm and slow feed are not good as they produce to much heat.
I set my spindle RPM down, ran a bit faster, and voila, it actually started chipping away and stopped pulverizing.
However, I would not have done that without the formulas and insight as the speed is rather scary now.
That little TAIG mill is flying through that stuff. I bought one of those contact free thermometers which look like a gun a couple of years ago and never really used that. Now I took it and measured the temp of the bit's shank during operation. Just for fun... I am not such a stickler usually. And.... it does show. Funny, I tended to do the wrong thing, as in high rpm low feed, as I thought it would make it easier on the cutter. Wrong. Now it's flying, cool, without squeaking which it did a bit before.
Just Great!
Thanks again!
Lemo

[Chaoticone]

Lemo, check this out, it might help as well. Although if they don't agree with Grahams, take Grahams word. He is a Gcode Guru.

http://www.wadeproco.com/

Brett