# Calculating Cutting Conditions for Milling Cutter Machining: Key Points to Remember

1. Question

What methods are available for calculating the cutting conditions for end milling?

In preparation for end milling, I referred to the cutting conditions table but couldn’t find the corresponding conditions for the desired machining.

What is the calculation method for milling conditions?

The spindle speed is calculated based on the milling speed; the feed rate is calculated based on the feed per tooth; the depth of cut is derived from the cutter diameter.

The spindle speed is calculated from the cutting speed and cutter diameter, with the cutting speed referenced from the cutting conditions table or machinability index.

The feed rate is calculated based on the feed per tooth, spindle speed, and the number of cutter teeth. The depth of cut is derived from the cutter diameter. Carry out machining tests based on the calculated results to adjust the milling conditions.

Method for Calculating Spindle Speed

Formula for Calculating Rotational Speed:

N=(1000*Vc)/π*Dc

Formula for Calculating Milling Speed:

Vc=(π*Dc*N)/1000

• N: Revolutions per minute (min-1)
• Vc: Milling speed (m/min)
• Dc: Cutting diameter (mm)

I. When the tool diameter used is not recorded in the cutting conditions table

You should calculate the milling speed based on the milling conditions of the closest diameter, using the formula given. Then, compute the rotation speed. A more straightforward approach is to use the desired diameter as a reference, and calculate the rotation speed by multiplying it with the ratio of diameters.

Figure 2 Cutting conditions table

For instance, when calculating the rotational speed of an end mill with a blade diameter of 2.8 for machining structural carbon steel,

The rotational speed of an end mill with a blade diameter of 3 is 7250 (min-1),

Hence, the rotational speed of an end mill with a blade diameter of 2.8 is: 7,250(min-1)×3/2.8= approximately 7,768(min-1).

*Under a constant milling speed, the smaller the blade diameter, the higher the rotational speed.

2. When the material to be machined is not listed in the cutting condition table,

It is calculated by multiplying the rotational speed of other listed machined materials by the ratio of the machinability index between the materials to be cut.

For example, when calculating the rotational speed of an end mill with a blade diameter of 3 for machining gray cast iron,

The rotational speed when the blade diameter is 3 and machining structural carbon steel is 7,250(min-1).

When the machinability index of structural carbon steel is 70 and that of gray cast iron is 85,

The rotational speed when milling gray cast iron is: 7,250(min-1)×85/70= approximately 8,804(min-1).

※ The machinability index is a value expressing the ease of machining materials, with the ease of machining free-cutting steel set as 100. The smaller the value, the harder it is to machine, and it can serve as a reference when setting the cutting speed.

Key points for setting the rotational speed

【When using a ball end mill】

When using a ball end mill, calculating based on the actual cutting diameter will be closer to the actual machining conditions.

Figure 3 Method to Calculate Actual Cutting Diameter and Correct Rotational Speed

1. When Spindle Speed is Limited

If the spindle speed is constrained by the machine tool, resulting in a slower processing speed than specified in the cutting condition chart, the feed rate should be reduced proportionally.

For example, if the recommended cutting conditions are a spindle speed of 30,000 (min-1) and a feed rate of 600 (mm/min), and the machine tool’s speed limit is 20,000 (min-1), then the feed rate will drop to 600 x 20,000 / 30,000 = 400 (mm/min). Moreover, the cutting speed can be maintained despite the reduced spindle speed by increasing the cutter diameter.

2. When Vibration Measures are Adopted

Even when the spindle speed is lowered to avoid vibration and prolong tool life, the change in cutting resistance within the common cutting speed range (for example, 50~150 (m/min) for carbon steel used in machine structures) is minimal and does not enhance efficiency.

Adjusting the depth of cut and feed rate is more effective. However, if vibration occurs at the inherent speed due to machine tool aging or if the workpiece is machined without knowing the correct cutting speed, the spindle speed should be adjusted.

See also  Unveiling the Mystery: Why Machine Tool Prices Aren't Marked Clearly?

Calculation of Feed Rate

The formula for calculating the feed rate is:

F=fz*N*Zn

The calculation formula for each cutting depth is as follows:

Fz=F/(Zn*N)

• F: Feed Rate (mm/min)
• fz: Feed Per Tooth (mm/tooth)
• N: Spindle Speed (min-1)
• Zn: Number of Teeth

1. When the Cutting Conditions Table does not list the corresponding conditions for the tool’s cutting edge diameter:

When calculating with the chip load per tooth as a constant, the chip load per tooth should be computed based on the speed and feed of the closest cutting edge diameter, and then the feed rate should be calculated using this value along with the machining speed.

In actual applications, changes in the cutting edge diameter and length will affect the rigidity of the tool. This must be taken into account when calculating the chip load per tooth. For basic usage, calculations can also be done based on the median values of the parameters listed in the Cutting Conditions Table.

Figure 5: Cutting Conditions Table

For instance, when using a vertical milling cutter with a blade diameter of 2.8 to process structural carbon steel, we’ll calculate the feed rate of the vertical milling cutter as follows:

Given that the feed speed is 360 mm/min when the blade diameter is 3 and 340 mm/min when the blade diameter is 2.5, the feed speed when the blade diameter is 2.8 would be: (360-340) / (3-2.5) * (2.8-2.5) + 340, which equals approximately 352 mm/min. The spindle speed is calculated using the “Spindle Speed Calculation Method”.

2. When the workpiece material is not listed in the cutting condition table:

The feed speed for the unlisted workpiece material is calculated by multiplying the feed speed of another listed workpiece material by the ratio of the machinability index between the two materials.

For example, when calculating the feed speed of a vertical milling cutter with a blade diameter of 3 when machining gray cast iron, the feed speed when machining structural carbon steel is 360 mm/min. The machinability index of structural carbon steel is 70, and that of gray cast iron is 85.

Therefore, the feed speed when milling gray cast iron becomes: 360(mm/min) * 85/70 = 437(mm/min). The spindle speed is calculated using the “Spindle Speed Calculation Method”.

## Key Points for Setting Feed Speed:

1. When taking vibration prevention measures:

For vertical milling cutters with long blade lengths that are prone to vibration, or those with long necks and large protrusions, or thin-blade-diameter types, reducing the depth of cut or feed per tooth can proportionally decrease the cutting resistance. Therefore, this is more effective than reducing the spindle speed.

Figure 6 shows a schematic diagram of cutting with a long-neck vertical milling cutter.

Furthermore, when machining the corner areas in lateral processing, the contact length of the cutting edge increases, so measures to reduce the feed rate are necessary.

Too small a feed per tooth can accelerate wear. Except for end mills with a fine diameter (less than 2), the feed per tooth should not be less than 0.01mm.

Figure 7: Schematic Diagram of Corner Area Machining

Calculating the Feed Rate

1. When Using an End Mill

Figure 8: Cutting Conditions for an End Mill

Figure 9: Depth of Cut in Side Machining

Figure 10: Depth of Cut in Groove Machining

The infeed amount Ad and Rd are calculated by multiplying the cutter diameter with the coefficient in the cutting condition table. For instance, when the cutter diameter is 5, and side milling is being performed, according to the cutting condition table, Ad is 1.5D and Rd is 0.1D. Therefore, Ad is 1.5×5, which is less than or equal to 7.5(mm), and Rd is 0.1×5, which is less than or equal to 0.5(mm).

2. When using a ball nose end mill

Table 11 (a) Cutting Conditions for Ball Nose End Mill

Table 12 (b) – Cutting Conditions for Ball Nose End Mills

Figure 13 shows the cutting depth Ad when using a ball nose end mill.

(a) When using a ball nose end mill, the cutting depth Ad is calculated by multiplying the tool diameter by a certain coefficient. For example, when the tool diameter is 2 and Ad is 0.1D, the calculation is 0.1 x 2 = 0.2(mm).

(b) When using the cutting condition table for ball nose end mills, the cutting depth Ad is directly read from the table. If the cutting conditions for the tool you wish to use are not listed in the table, please use the middle value of the closest tool diameter and effective length.

3. When the material to be machined is not listed in the cutting condition table

Use the mechanical structural carbon steel or tempered steel listed in the cutting condition table as a baseline.

For materials softer than the baseline, temporarily set the cutting depth to the same value and increase it to a level where no problems occur through trial machining.

For harder materials, set the value to the cutting depth multiplied by the ratio of the machinability index of the two, and perform test machining.