Manufacturers of cutting tools typically provide recommended cutting speeds for their products. However, these values are broad estimates based on ideal conditions, such as rigid setups, annealed materials, and the most suitable carbide grades. In reality, these conditions are rarely met, making it necessary to adjust the recommended speeds to fit specific applications. This article will guide you through the process of making these adjustments effectively.

Another useful application of these guidelines is when you have an established cutting speed that works well in a given scenario, but one or more parameters – such as material hardness or stability – change.

Although Speeds and Feeds calculators can perform the task, a solid grasp of the fundamental variables involved will allow for more informed and precise decisions.

Fig 1 – Hardness vs Speed

Identifying the raw material
Most cutting tool recommendations can be found on product packaging or in supplier catalogues, both in print and online. However, the data provided on packaging groups materials into the six broad ISO categories (P/M/K/N/S). On the other hand, supplier catalogues provide more detailed classifications, often with 40 to 100 material subgroups.

Since there is no industry-wide standard for categorising materials, each supplier has its own classification system. Therefore, it is crucial to invest time in accurately identifying your material according to the supplier’s system before proceeding. Skipping this step can lead to significant errors.

Another viable approach is to use past experience with similar materials as a reference point and apply adjustments based on the factors outlined below.

Fig 2 – Stability Speed Factors

Fig 3 – Taylor Tool-Life

Adjusting for material hardness
In some instances, you may have data for a material in its annealed state, but the actual workpiece requires machining after heat treatment. A common example is precipitation-hardened stainless steels or high-alloy steels.

To modify the cutting speed accordingly, refer to the chart in Fig 1. The X-axis represents the difference in Brinell hardness between the reference material and the actual workpiece, while the Y-axis shows the percentage of speed adjustment required.

Evaluating setup stability
The overall stability of a machining setup significantly impacts the appropriate cutting speed. Stability is a subjective measure influenced by factors such as the rigidity of the workpiece and tool clamping, as well as tool overhang.

To assess stability, rate the setup on a scale from 0 to 10, where 10 represents an ideal scenario with minimal tool overhang, and zero indicates a highly unstable setup. Most cutting speed recommendations assume a stability level of around 8. If your setup deviates from this, adjust the speed accordingly using the guidelines in Fig 2.

While this evaluation is somewhat subjective, it provides a useful framework for understanding how stability influences cutting speed optimisation.

Balancing tool life and productivity
There is no absolute “correct” cutting speed – only a range of values that balance productivity and tool life. Higher speeds enhance productivity but reduce tool life, whereas lower speeds extend tool life at the cost of productivity. The appropriate choice depends on your priorities. A widely used model to describe this relationship is the Taylor Tool Life Equation:

(V1/V2) = (T2/T1)^n

Where:
• V1 = Initial cutting speed
• V2 = Adjusted cutting speed
• T1 = Initial tool life
• T2 = Adjusted tool life
• n = Material-dependent constant

For carbide tools, n typically falls between 0.2 and 0.4, depending on the material and grade. In Fig 3, a Taylor model graph with n set at 0.3 demonstrates how cutting speed affects tool life. For instance, reducing speed by 50% can extend tool life up to tenfold, while increasing speed by 50% can reduce tool life by 75%.

While exact values differ between materials, the key takeaway is that cutting speed has a major effect on tool life.

Considering radial depth in milling
In milling operations, radial depth of cut (Ae) is an important factor. When Ae is smaller than the cutter’s radius, chip thinning occurs, allowing for an increased feed rate. However, fewer people recognise that this also permits an increase in cutting speed.

Fig 4 – Radial Depth

Fig 5 – Radial Depth Speed Factors

A lower radial depth means each cutting edge spends more time outside the material, improving cooling and allowing for higher speeds (as shown in Fig 4). The extent of this speed increase depends on the cutter’s diameter and the Ae/d ratio (radial depth divided by cutter diameter).

Most supplier recommendations assume an Ae/d of 0.5, meaning the radial depth equals the cutter’s radius. To determine the appropriate speed adjustment, refer to the table in Fig 5.

Conclusion
The principles discussed in this article are not pure science. However, applying them correctly allows for more precise and efficient adjustments to cutting speeds based on real-world conditions.

This is the viewpoint of Erez Speiser, Founder and Owner of the Machining Doctor. For more information visit https://www.machiningdoctor.com