Cutting Speeds: From General Recommendations to Real-Life Values
All cutting tool suppliers provide recommendations for the cutting speed of their products. However, these suggestions are quite broad and intended for near-perfect conditions like stable clamping, annealed material, and ideal carbide grade. As a result, these recommendations are too high in many situations, and we need to adjust them to our specific application. This article will teach you how to make these adjustments professionally.
Another practical use for the tips presented in this article is when you have a cutting speed that works well in specific conditions, but one of the parameters (e.g., material hardness, stability) changes.
You can use speeds and feeds calculators to make these calculations automatically. However, having a solid understanding of the fundamental parameters that influence the calculations will enable you to make much better decisions!
Raw Material Identification
The recommended cutting speeds for a product are usually available in product boxes and catalogs (Print and online). It is advisable to ignore the speed recommendation on the product boxes. The reason for this is that the information on the product boxes is usually limited to the six main ISO material groups, whereas the classification in the catalogs is much more detailed and specific.
Supplier catalogs usually have multiple subgroups within each group. However, there is no standardization among the different suppliers, and each created its own list of material groups. Typically, a list will have around 40 to 100 sub-groups.
It is critical to invest adequate time in classifying your material correctly according to the supplier of the cutting tool you will be using before moving on to the next step. Although this process may be time-consuming, it is not the place to take shortcuts!
Now that we have the most accurate starting point, let’s move on to the following steps to fine-tune.
Another option is to use your prior experience with a similar material to determine the starting point and manipulate it using the guidelines below.
Raw Material Hardness
In some cases, you may have experience or cutting speed recommendations for a material in its annealed condition, but it must be heat-treated before machining. A typical example is PH stainless steels or high alloy steels.
To adjust the cutting speed, refer to the chart on image #1. The X-axis displays the hardness difference in Brinell units between the material you are working on and the material for which you have the original data. The Y-axis indicates the percentage of adjustment needed to apply to the basic cutting speed.
The appropriate speed for a machining application is largely determined by the overall stability of the setup, which is a subjective assessment. It depends on the quality of the clamping of both the workpiece and the cutting tool, as well as the overhang of the cutting tool. To assess your application’s stability, rate it on a scale of 0 to 10, where 10 represents a perfectly stable setup with a short tool overhang, and 0 represents a poor setup in terms of stability. Assume that the catalog recommendation is for a score of 8, and adjust the speed according to the factors from the chart provided in image #2.
It is important to note that this is a subjective estimation. However, it is a helpful outset for understanding how stability affects cutting speed tuning.
Tool-life Vs. Productivity
The conceivable cutting speed range to use is quite broad, and there is no right or wrong choice here. Opting for a higher cutting speed will increase productivity but reduce tool life, while a lower speed will extend tool life but decrease productivity.
The approach depends on your targets and personal preferences. There are several models for the relation between cutting speed and tool-life. The most commonly used is the Taylor model:
V1=Current cutting speed
V2=New cutting speed
T1=Current tool life
T2=New tool life
The value of n for carbide grades typically falls between 0.2 and 0.4 and depends on the grade and raw materials used.
In image #3, you can see a plot of the Taylor model with n=0.3
The chart shows that a 50% reduction in cutting speed can increase the tool life up to 10 times. On the other hand, increasing by 50% can reduce it by 75%. Although the numbers vary for different materials, the main takeaway is that the cutting speed has an exponential impact on the tool life.
Radial Depth (Milling)
In milling operations, there is another factor to consider, and that is the radial depth of cut (Ae).
When the radial depth is lower than the cutter radius, the feed rate can be increased because of the chip thinning formula. However, fewer people know that the cutting speed can also be increased. We can increase the speed since a smaller radial depth allows more time for cooling outside the material for each flute (See image #4). The amount we can increase depends on the cutter’s diameter and the ratio between it and the radial depth (Ae/d). You should assume that the starting point recommendation is for Ae/d=0.5 (The radial depth equals the cutter’s radius). Now, you can use the table in image #5 to get the speed adjustment factor.
Please note that the information provided in this article is not pure science. However, it can be helpful in fine-tuning cutting speeds according to changes in your application.
About the Author
Erez Speiser is the founder and developer of the Machining Doctor Website. The platform encompasses his 30 years of experience in the machining industry, during which he held managerial positions in Engineering, Production, and Marketing. Combining his extensive knowledge of the industry and web development skills, Erez founded the Machining Doctor – a platform that serves as a hub for industry professionals to access his wealth of expertise and insights. Contact him on LinkedIn.