[FoxCNC1]

Hi guys, im was never able to understand how to calculate feeds and speed for drilli g opeartions on a mill or cnc machine.

I am family with how horizontal feeds and chipload work, but does any of this apply to drilling?

I have drill several holes (hundreds) that make a patters. The holes are 1/8" in diameter so rather than trying to mill them it would be faster to just drill.

Any information would be helpful.

[KnuckleBuster]

How deep? What machine? What material? Do you have TSC?

[FoxCNC1]

Alum. 1/4 with a 1/8 2 flute drill.
What is TSC?

[deadlykitten]

I am family with how horizontal feeds and chipload work, but does any of this apply to drilling?

hy it does not matter if it is a drill, a face mill, or a turning tool, etc : formula's apply to the cutting edge ( geometrical location )

let's calculate a few examples :

1) drilling ( on mill or lathe, rotating tool or rotating part ) a 32mm hole with 100M/min means that rpm has to be 100*320/32=1000 rot/min; feed may be 0.1mm/rot or 1000*0.1=100mm/min, depending if you like to use feed in mm/revo or in mm/min

G97 S1000 M03 M08
G00 X0 Z2.5
G01    Z-50 F0.1 G95 ( or F100 G94 )
       Z-50+0.3
G00    Z2.5

2) face milling : tool dia 250 with 12 teeths; required rpm for 75M/min is 75*320/250=96 rot/min ( thus, this won't run on a cnc mill, but on a classical mill, because it has torque at low rpms ); feed may be 0.1mm/tooth, thus 12*0.1=1.2mm/rot or 96*1.2=115mm/min

depending on machine rigidity, you may start to increase ap & ae

3) turning diameter 90mm at 150M/min requires 150*320/90rot/min; feed may be, for example, between 0.05 - 0.70mm/revo

4) grinding calculations begin with computing rpm for the grinding wheel, and the part is simply feed ( moved or rotated under it )

1/8 2 flute drill

1/8=cca3.2mm

in alu you may go twice as fast as in steel, or even higher; rpm for 100M/min is 100*320/3.2=10000 ... that's the math, at least theoretical

in reality, your tool may overheat pretty fast, and also depends how your machine spindle behaves at such speeds, and what is the machine limit and taper size

obviously, is better to have a low tir spindle and internal-coolant tool and an rpm limit > 20000, rather then a dull hss drill and a spindle limit of 9000 / kindly

ps : tsc : through spindle coolant
ps2 : i understand "chipload" as required spindle torque / cutting edge, while in reality it means feed/cutting_edge ... a proper name should be chipthikness ... you see, there is an adaptive okuma function, that is capable of delivering identical spindle torque by modifing chipthikness for each cutting edge : for example, if you use a face mill with 6 teeths that has tir, then each tooth will cut a different chipthikness because tir<>0, thus spindle torque for each tooth will be different; if the adaptive function kicks in, then feed will be automaticall adjusted ( with a rate of 6 times/revolution ), in order to stabilize the cutting, making it behave like the tool had low tir

[FoxCNC1]

Thank you , What is the 320 number so that I can try to convert your formula to imperial?

[deadlykitten]

is an aproximation of 1000/pi

use the internet to find out the math behind this ... should help you to understand what is behind

there are many that simply use the formula "as it is", without wondering why it works ... is better to know those details, and also to be able to switch fast between feed in mm/revo and mm/min

if you wish, i will be back with explanations, or maybe someone has a link to something sugestive

---

let's consider that you have a wheel at your car that is 300 [ mm ]

what rpms to input, in order to achieve a speed of 100 [ M / min ] ?

and here it is :

    circumference of the wheel is 300 * pi [ mm ]
    V = 100 [ M / min ] = 100 * 1000 [ mm / min ]
    rpm = V / circumference = ( 100 * 1000 ) / ( 300 * pi ) [ [ mm / min  ] / [ mm ] ] = 100 * cca320 / 300 [ 1 / min ] = cca107 [ rpms ]

thus, for a tool of diameter D, in order to achieve a tangential speed of V ( normaly listed on the label of the insert box ), one should input an rpm of V*320/D

as you can see, 1000/pi is not exactly 320, so this means that one can be tolerant with the given cutting specs, and should not follow them exactly, but only as a reference

in time, each develops it's own specs, and some guys never go over a specific spindle load, others are in a hurry, or like to rush / kindly

[g-codeguy]

Alum. 1/4 with a 1/8 2 flute drill.
What is TSC?

I am going to assume Through Spindle Coolant. As deadlykitten said it matters not if a drill or turning. Formula is the same. It does matter if it is metric or not. I don't use metric. My formula is RPM=12*sfm/pi*dia or shortened version 3.82*sfm/dia

[jaibros]

Yes, the principles of feeds and speeds also apply to drilling operations on a mill or CNC machine. In drilling, the key parameters that affect cutting performance are spindle speed, feed rate, and the type of drill bit being used.

To calculate the optimal feeds and speeds for drilling, you can use the following steps:

Determine the type of material you will be drilling into, as this will affect the hardness of the material and the type of drill bit needed.
Identify the recommended surface footage (SFM) for the material being drilled. This is the speed at which the material is moving past the drill bit and is typically given in surface feet per minute.
Use the formula: RPM = (SFM x 3.82) / drill diameter to calculate the recommended spindle speed in revolutions per minute (RPM).
Determine the recommended feed rate based on the diameter of the drill bit and the material being drilled. A general rule of thumb is to use a feed rate of 0.001 to 0.004 inches per revolution (IPR).
Adjust the speeds and feeds as needed based on the specific conditions of your drilling operation, such as the depth of the hole, the coolant being used, and the rigidity of your setup.
It's important to note that drilling can generate a significant amount of heat, which can cause the drill bit to wear out quickly. To prevent this, it's important to use a coolant during drilling and to periodically check the condition of the drill bit to ensure it is still sharp and functioning properly.

I hope this helps you in calculating the feeds and speeds for your drilling operations!

https://jaibros.com/products/u-drill1-mm