CNC programmers do not directly include the tool nose radius in the program, as the toolpath uses drawing dimensions and the actual radius is handled by cutter radius offset. That does not mean the programmer should totally ignore the corner radius or even the back angle of the selected tool.

The most commonly used corner radiuses for turning and boring are 0.4 mm, 0.8 mm, and 1.2 mm or their Imperial equivalents of 1/64, 1/32, and 3/64. The middle size (0.8 mm or 1/32 inch) is the most common radius used, but that also depends on the machine size and the type of work. Typically, larger radiuses (up to 1.6 mm or 1/16 inch) are common for large CNC lathes with higher power rating. Large radiuses are also selected for heavy work on castings and forgings, to minimize tool wear. In addition, it is not just the nose radius itself that has to be considered, but the insert size as well. The larger the inscribed circle of the insert (as per tooling catalog), the heavier cut may be taken, providing the machine has enough power to handle it (power is measured in kW or HP).

The above illustration shows an example of a 80° insert with 0.4 mm radius (0.0156 inch) and a 5 _ back angle, as well as a 55 _ insert, also with a 0.4 mm radius but 32 _ back angle. At the common feedrate of F0.25 mm/rev (0.0984 in/rev), note the depth of the scallops caused by each tool in millimeters. The following metric and Imperial tables show the differences for all three common radiuses:

The example shows quite clearly that selecting the turning or boring tool based on radius alone is not always sufficient, particularly if a certain surface finish is to be achieved. There is a clear relationship between the tool nose radius, the back angle and cutting feedrate.

Every machinist knows that a larger corner radius provides a better surface finish as compared to a smaller corner radius under identical conditions. The reason is that a smaller corner radius will develop a deeper ridge than a larger corner radius - again, under identical cutting conditions, as demonstrated in the tables.

Selecting the proper corner radius for a particular turning or boring operation should take a few realities for consideration:

• Smaller radius has much smaller inclination to cause chatter than a large corner radius
• Chip formed by a smaller corner radius is more uniform than a chip formed by a large radius
• Rigid setup, including a strong tool holder, increase in importance for larger corner radiuses
• Material support is important, particularly for a large stock extension to stock diameter ratio
• Internal corner radius is not the only reason for small corner radius - small radius is better for thin material
• Smaller corner radius is also beneficial for longer stock extension (such as 1:4 or 1:5 diameter to length ratio)
• Tool life increases for inserts with greater included angle

These are just some of the observations determined by the tooling companies and actual users. Sometime it may take a bit of an experimentation to select the best toll - and corner radius - but it also shows that a corner radius selection should be considered as carefully as making other decisions.

Cutter radius offset is also known as the tool nose radius offset on CNC lathes. Its purpose and overall functionality is the same as for milling applications and has been described in great detail earlier, in a separate chapter ' Using Cutter Radius Offset' . This section will only cover some additional items important for lathe applications, mainly the effect of not programming cutter radius offset.

Surprisingly, a significant number of machine shops do not use cutter radius offset on CNC lathes at all or using it poorly. Regardless of the reasons (some are mere excuses), the message is simple – in manual programming you do need to compensate for the tool nose radius. If you don't, the finished part just will not have the right dimensions - it can't have.

The main reason is the method of setting up the tools for turning and boring. In majority of setups, the mounted tool is touched-off the Z0 face to get the Z-axis geometry offset. The same approach is applied to the X-axis as well, but since it is impossible to touch the center line, the measuring process takes some extra steps, but the final result - the X-axis geometry offset - is the same as if the center line could had been touched. Both measurements are made between the extremities of the tool tip and the X0 or Z0. In practice, it means there is a significant difference between setting the radius offset for milling applications and doing the same for turning and boring applications. Rather than the center of cutter radius (as in milling), the lathe setup (geometry offset) is measured to a corner point of the tool nose, often called the imaginary tool point or the virtual tool point .

The illustration shows the offset measurement for both axes, as well as their effect on a diameter cutting (Z-only direction) and the face or shoulder cutting (X-only direction). When it comes to cutting radiuses, chamfers and tapers, the control system requires a different type of internal calculations, therefore it also requires a few adjustments in the programming (and setup) method.

Imaginary Tool Point

In the illustration at right, three points are shown as examples of imaginary points of typical lathe tools. These three points have one thing in common – they both are the only setup points the controls system 'knows about' . These points are often called the command points , as they are commanded by the program. Each XZ coordinate in the program determines the actual position of the command point on the contour.

Position of Command Points on a Contour

A typical contour is not just a series of diameters and faces, it also includes radiuses, chamfers and tapers. Without cutter radius offset, the command point will always be positioned at the endpoint of the contour element. As the illustration on previous page shows, there is no problem with diameter or face cutting. The illustration below shows the position of the command point at the end point of a radius, chamfer or a taper, in different configurations. Only an external contour is shown, but it applies equally to an internal contour as well.

Without a cutter radius offset, either excessive cutting or insufficient cutting will take place, resulting in dimensions that do not conform to the drawing.