Hello Guest it is September 25, 2023, 05:27:13 AM

### Author Topic: How fast can I go? Safely...  (Read 3758 times)

0 Members and 1 Guest are viewing this topic.

#### lemo

• 135
##### How fast can I go? Safely...
« on: May 22, 2007, 07:22:56 PM »
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

Cut five times and still to short...

#### Graham Waterworth

• 2,621
• Yorkshire Dales, England
##### Re: How fast can I go? Safely...
« Reply #1 on: May 23, 2007, 03:33:58 AM »
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.
Without engineers the world stops

#### lemo

• 135
##### Re: How fast can I go? Safely...
« Reply #2 on: May 23, 2007, 09:57:13 AM »
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
Cut five times and still to short...

#### Chaoticone

• 5,624
• Precision Chaos
##### Re: How fast can I go? Safely...
« Reply #3 on: May 23, 2007, 11:04:26 AM »
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.