In a machining environment, stock allowance is a term that defines the amount of material left for finishing after rough cutting had been completed. Although it seems a subject simple enough to ignore, there are some considerations that will influence the programming techniques applied to roughing, particularly the last tool passes, where the stock will applied.

The major considerations of stock selection and control are the nature of the cut, particularly the shape of finished contour, and the type of tool used. Leaving stock on the roughed contour is generally designed for the finishing cut, but there could be other reasons, for example, as a grinding allowance. When using the G71/G72 lathe cycles, stock allowance can be defined in the cycle. If a cycle is not used, the required stock allowance must be programmed directly, even if it means a few additional calculations.

Contour Shape

Most contour toolpaths will be a combination of lines and arcs, where the lines represent diameters, faces, shoulders, tapers and chamfers, while arcs represent fillet radiuses, partial radiuses, undercuts, etc. Stock left on an external contour will increase its nominal size, whereby stock left on internal contour will decrease its nominal size.

Cutting Tool Used

A typical cutting tool (external or internal) used on a CNC lathe may have several tip orientations, depending of the tool design and its direction when mounted in the turret. The standard turning and boring tools (with 80 _ , 55 _ , 35 _ inserts) mounted for typical working conditions are the ones to watch for. The main problem is with their front clearance angle (lead angle), particularly when a face or a shoulder is machined. Unlike in conventional machining, where tool cutting direction can be changed frequently, on a CNC lathe the situation is different, particularly when using lathe cycles. Tool cutting direction can change as per programmer's decision, but not with cycles. Both G71 and G72 (and G70) maintain a uniform toolpath and changing direction is rather limited. It is possible to program part of a contour using G71 cycle, and another part using the G72 cycle.

Stock Allowance in X and Z axes

Having a uniform stock over the whole contour is not only impractical, it can even be dangerous. This is no overstatement and the reason is the tool geometry and its use in the part program. Typical lead angle for 80 _ inserts is 5 _ , while the lead angle for 55 _ and 35 _ inserts is 3 _ . When facing up, the edge of the tool is almost parallel with the face, leaving virtually no clearance. When the stock on the face is too heavy, the insert can literally be 'buried' in it and cause severe problems. The solution is to leave the Z-stock very small - see below.

Both the G71 and G72 cycles allow stock allowance specification to be selected individually for the X-axis and the Z-axis. Depending on the type of G71/G72 cycle, the format is either a single block or a double block:

• Single block format:

G71 P.. Q.. I.. K..       U.. W..             D.. F.. S..         U and W are stock allowances

G72 P.. Q.. I.. K..       U.. W..             D.. F.. S..         U and W are stock allowances

• Double block format:

G71 U.. R..

G71 P.. Q..      U.. W..             F.. S..               U and W are stock allowances

By definition, the U-address is the stock left on the diameter in the positive or negative direction, while the W-address is the stock left on the faces or shoulders in the positive or negative direction. On a rear type lathe, typical U-address will be positive for external cutting and negative for internal cutting. For the majority of jobs, the W-address will be positive for both external and internal toolpaths.

The U-address for stock allowance is always measured on the diameter !

The actual amount of stock left on diameters will depend to a large extent on the type of job, material, tool nose radius and general setup. For thin or tubular stock, a smaller amount of stock may prevent chatter during finishing, particularly when combined with a smaller tool nose radius. If cutting conditions are favorable, stock allowance per side is commonly programmed close to the tool nose radius. For example, U1.6 will leave 0.08 mm of stock for finishing, per side. In Imperial units, similar stock allowance would be programmed as U0.06, leaving 0.03' per side for finishing.

As the illustration on previous page shows, when cutting with G71 cycle, the facing will be in the up direction, and the W stock allowance must be very small, typically between 0.08 to 0.15 mm or 0.003 to 0.006 inches. With such small amounts, the tool lead-in angle does not produce heavy depth of cut. There is way to calculate the actual depth of cut on a face, using the following formula:

Compound Stock

When the stock allowance on diameters is combined with the stock allowance on faces, the actual stock allowance is equivalent to neither the U nor the W amount of the G71/G72 cycle - it becomes a compound stock . In simpler terms, compound stock is a combination of the U and W amounts applied to angles and radiuses. The illustration shows a typical compound stock ©). Although the programmer should be aware of its existence, there is no reason to pay special attention to compound stock in daily programming.

Grinding Allowance

Leaving stock for subsequent turning or boring operations is the most common application of stock allowance. In some cases, no stock is left on the part for turning or boring, but for grinding - this is a somewhat different type of stock allowance, called grinding allowance . Neither G71 nor G72 cycle supports grinding allowance as such, although it can be used for such purpose in certain cases.

A true grinding allowance is a suitable amount of stock left for the sole purposes of grinding on selected diameters and/or faces and shoulders. The key word here is selected entities, as compared to all entities for turning or boring. Take - as an example - the drawing shown at right (sizes are not to scale and exaggerated for clarity) - the diameter will be ground later, after the CNC lathe machining is completed. The taper that precedes the diameter is turned to size - it is not ground. For a smooth transition between the finished taper and the unfinished diameter, the taper should be extended. Programmer selects the amount of grinding allowance, in this example as 0.05 mm (~0.002").

The taper (or a chamfer) extension can be easily calculated, based on the grinding allowance G and the taper (chamfer) angle A , using simple trigonometric function:

This extension will be added to a known Z-axis location, as defined in the drawing between the taper and the finished diameter (not shown). At the same time, the specified drawing diameter will be increased by the double grinding allowance G (or decreased for boring). The effect on the part face (shoulder) was not considered in this example.

In many cases, there will be some radius required in the corner between the part diameter and the face or shoulder. In this case, a smooth transition is required, so a new radius has to be programmed - a temporary one for the grinding allowance. Note that the grinding allowance is applied to the diameter only, not the face.

The center of the temporary radius r has to be shifted from the center of the defined radius R by the amount of grinding allowance G . Also, the temporary radius r must be smaller than the defined radius R, by the amount of grinding allowance G .

Both of the presented examples are quite easy to calculate. The main focus is to correctly evaluate the engineering or production demands in terms of grinding allowance requirements.

Series of tool motions programmed before the first element of the contour is machined is called tool approach or lead-in motion. When the tool approaches the contour, it can approach a face, diameter, chamfer or a taper, or a radius. A series of similar drawings shows the main features of a tool approach towards a part (not to scale for clarity). Note that the approach direction is only an example, and can originate from another point.

Approaching the Front Face

In most turning jobs, there will be a need to program at least one facing cut, to remove the front face stock. The tool should start well above the stock diameter by a clearance C of 2.5 mm (or 0.1 inches) per side - or more, if necessary. Keep in mind that not all parts are perfectly round and the rotation increases the effective stock diameter. Using cutter radius offset for the face alone is nor necessary, but will do no harm if programmed correctly.

Approaching a Diameter

Any tool motion towards a diameter is the easiest to program and requires no special considerations. It is similar to the previous example, except for the cutting direction. For both external and internal cuts, the tool should have a suitable clearance from the part, along the Z-axis. Typical clearance C of 2.5 mm or (0.1 inches) is generally sufficient. Cutter radius offset should always be in effect, even for the simplest of contours. The approach motion is also the motion that activates cutter radius offset for turning or boring.

Approaching a Chamfer

Many contours start with a chamfer or a taper. Approach towards a taper is a little more involved and has been defined in detail in the chapter Programming Tapers . Chamfers are much more frequent as the first entity of a contour. In order to maintain the angle of the chamfer, the cutting tool has to approach the part at a selected Z-axis clearance and a calculated X-axis diameter. Cutter radius offset should always be in effect for precision machining.

Approaching a Radius

If the first element of the machined contour is a radius, the tool approach is unique in the sense that it must include two motions during the lead-in. The reason is that cutter radius offset (which should become effective during the approach) cannot be started on an arc. That means a lead-in linear motion must be programmed first, and during this motion the radius offset will be activated.

There are three typical approach methods to an arc, all shown here with examples. All methods are similar, whether tool moves towards a tangential arc or an intersecting (partial) arc. This section explains typical programming techniques of approaching an arc as the first entity of a finished contour.

For the next example, the initial tool approach will also be towards a tangential radius, but located

not at a corner, but at the centerline. This type of radius is called spherical radius .

Another radius that can be the first element of a finishing contour is an intersecting arc , sometimes

called a partial arc

The first calculation must be the diameter at the intersection. Once this diameter is known, the starting diameter can be calculated very easily.

Pythagorean Theorem method will be used to calculate the dimension W . Once the W dimension is known, the unknown diameter _ X can be calculated by subtracting the double amount of the lead-in arc from the new diameter.

From the examples shown, the various methods of programming a tool approach towards a part, generally for finishing operations, should be clear. It is impossible to cover all possibilities, but these representative examples show the most common situations. One common denominator should be apparent from all the previous examples:

Approaches to Avoid

The following illustration shows what tool approaches to avoid. In all cases, the G42 command (or G41 for boring) is activated during the approach towards the part.

One main reason for the avoidance is to prevent improper application of the cutter radius offset. The bottom left image will be used as an example - see detailed illustration.

Although the cutter radius is applied correctly, and the Z-clearance is also correct, the tool tip approaches the chamfer at the same diameter as the lower chamfer point, resulting in an incomplete chamfer. The error will be greater when a large tool radius is used and will also be influenced by the chamfer (taper) angle. Compare with the correct approach methods shown earlier in this section.