Majority of tooling catalogues define the term 'deep grooving' as applicable to those grooves where the ratio of groove depth is 1.5 times greater that the groove width or higher. Selection of a deep grooving tool is determined not only by the groove width, but particularly by the groove depth . The grooving blade (insert) must be slightly longer than the groove itself, in order to provide all necessary clearances. Another very critical aspect of setting a deep grooving tool at the machine is the tool orientation - it must be perpendicular to the machine centerline, otherwise even a slight deviation may result in a distorted groove. Although correct tool setting is important for all grooves, it is much more important for deep grooves.

Deep grooves are often programmed using an interrupted cut, generally for the purpose of breaking the chips that may accumulate during machining. In the provided example, the deep groove is 18 mm deep. The grooving motion has to be interrupted every 6 mm, in order to clear the chips from the groove area. After each motion, the tool will retract 0.5 mm, before cutting the next 6 mm depth. If chip clogging is a problem (for some materials it can be), retract the grooving tool all the way above the part diameter.

The grooving insert selected for this job is 5 mm and can cut into the full depth of the groove. Based on the actual material and selected cutting conditions, the CNC programmer has to select the maximum depth of each cut . For this example, the depth of each has been selected as 6 mm, resulting in three 'peck' grooves (interrupted cuts) required to complete the groove to its full depth. Breaking chips on deep grooves provides two main benefits - increase of the tool life and better groove quality.

The programs above show two versions with the same result. The program on the left is more efficient as the retract after each cut is only 0.5 mm above the current diameter. This method is suitable if chipbreaking only is desired. The program on the right shows the tool retracting to the clearance diameter ( _ 54) after each cut, then returning to make another cut from 0.5mm above the last diameter.

G75 cycle could have been used for this example, but block-by-block method is more effective for understanding the program. If a corner break (chamfer) is required to eliminate burrs or the groove is wider than the insert, apply the method used in the 'Grooving for Precision' .

Pulley grooves described in the next section are special purpose grooves with tapered walls, used for very unique applications. There are many 'special purpose' grooves that do not have their two walls parallel with the machine axes. The most common of these grooves is a particular group of grooves called 'O-ring grooves'. This group also includes grooves with tapered walls, but with specifications unique to a particular industry or application. The purpose of the taper is to guarantee a high quality seal, as O-ring grooves are mainly used for the purpose of sealing, using a rubber ring or a similar sealing device. In this section, a typical approach to programming an O-ring groove is explained. Keep in mind that this technique can be used for any groove with tapered walls and corner radiuses. This section is not intended to cover the subject of O-ring grooves, only their programming.

The drawing at right shows a typical groove that belongs to this category. Common characteristics of such grooves are tapered walls, usually up to 5° for each wall, specified groove radius at the bottom diameter, groove corner breaks at the top diameter, and the groove width, provided as the distance between sharp corners.

The first step in the process is to select a suitable grooving tool – note that a standard grooving tool is used.

As the groove width is 6 mm, it may be tempting to select a smaller width grooving tool just by guessing. This is not a professional approach, and may backfire - the proper approach is to calculate the exact length of the flat area at the groove bottom. Besides, once this length is known, the calculation can be used to find the coordinate of the few points required in the program.

In the detail shown, only one half of the groove is required, as the other half is symmetrical by the groove centerline.

The first calculation is for the Z-value of point P1. Find the angle A, which is (90+5)/2=47.5°. As one side of the triangle is known, the other one can be calculated using trigonometric function. Once the Z1 dimension is known (calculated as 0.687248 mm), the flat of the groove bottom may be calculated as well:

Width of groove - 2 x Z1 = 6 - 2 x 0.687248 = 4.626 mm

Grooving tool selected must be smaller than the flat width, and 4 mm wide grooving tool seems like the choice - it will be used for the example.

Z-coordinate of the point P1 can also be calculated by simple subtraction. If the groove center is at Z-30.0, the left sharp corner must be at Z-33.0. By subtraction of Z1, P1 can be calculated:

P1 (Z) = -(33 - Z1) = -(33 - 0.687248) = -32.313 . . . . P1= X70.0 Z-32.313

Once all coordinates left of centerline are known, the corresponding coordinates at right are easy.

In order to calculate coordinates for P2, another calculation is necessary. The triangle to solve originates at the radius center, and the known hypotenuse of 0.75 is the radius.

Once the X2 and Z2 dimensions are known, the actual coordinates can be calculated as well.

P2 (X) = 70 + 2 x 0.75 - 2 x X2 = X71.369

From the previous calculation, Z1 is 0.687248:

P2 (Z) = -(33 - 0.687248 + Z2) = Z-33.060

P2 = X71.369 Z-33.06

The last calculations are for the corner break between the groove top diameter and the wall. The left corner break will be calculated next.

Both points P3 and P4 can only be calculated from a known point. Since the sharp point of the corner break is unknown, it must be calculated.

Disregarding both radiuses, the dimension Z3 can be calculated. Adding this calculation to the known sharp corner at the bottom, the coordinate point for the sharp corner at the groove top is:

X80.0 Z-33.437

Now, points P3 and P4 can be calculated as well.

The illustration at right shows both calculations, starting with the angle A. Note that once the dimension Z4 has been calculated, it will be used in both calculations. Once as the opposite side, then as the hypotenuse.

P3 (X) = 80 - 2 x X5 = 80 - 2 x 0.273853 = X79.452

P3 (Z) = -(33.437 - Z5) = -(33.437 - 0.023959)

= Z-33.413

P4 (Z)= -(33.437 + Z4) = -(33.437 + 0.274899)

= Z-33.712

Program coordinates for P3 and P4 are:

P3 = X79.452 Z-33.413

P4 = X80.0 Z-33.712

Even if it appears like a lot of work, keep in mind that the radiuses are necessary for O-ring grooves, as they provide a smooth surface for the seal ring. Fortunately, the coordinate points to the right of centerline will use the same calculations - apart from some additions and subtractions, there are no new calculations.

For easier reference, P11 is related to P1, P12 to P2, P13 to P3, and P14 to P4. Note that the differences are only along the Z-axis, while the diameters remain the same. Here is the complete list in the order of machining!

X80.0              Z-33.712          (P4)

X79.452          Z-33.413          (P3)

X71.369          Z-33.06            (P2)

X70.0              Z-32.313          (P1)

X80.0              Z-26.288          (P14)

X79.452          Z-26.587          (P13)

X71.369          Z-26.94            (P12)

X70.0              Z-27.687          (P11)

Complete program uses the points as defined, along with other program instructions:

(T06 = 4 MM WIDE GROOVING TOOL)

N1 G21

N2 T0600

N3 G96 S100 M03

N4 G00 Z-32.0 T0606 M08                           (GROOVING MIDPOINT AT GROOVE CENTERLINE)

N5 X82.0                                                        (1 MM PER SIDE DIAMETER CLEARANCE)

N6 G01 X70.2 F0.25                                      (0.1 MM LEFT ON GROOVE BOTTOM)

N7 G00 X82.0                                                (RETURN TO ORIGINAL START POINT)

N8 Z-33.712                                                    (POSITION OF LEFT CORNER BREAK - P4)

N9 G01 X80.0 F0.15                                      (START OF LEFT CORNER BREAK - P4)

N10 G02 X79.452 Z-33.413 R0.3 F0.1          (CUT LEFT CORNER BREAK - P3)

N11 G01 X71.369 Z-33.06 F0.15                   (LEFT TAPERED WALL - P2)

N12 G03 X70.0 Z-32.313 R0.75                    (LEFT GROOVE RADIUS - P1)

N13 G00 X82.0 Z-32.0                                   (RETURN TO ORIGINAL START POINT)

N14 Z-30.288                                      (* START OF RIGHT CORNER BREAK - P14)

N15 G01 X80.0                                              (START OF RIGHT CORNER BREAK - P14)

N16 G03 X79.452 Z-30.587 R0.2 F0.1          (* CUT RIGHT CORNER BREAK - P13)

N17 G01 X71.369 Z-30.94 F0.15                   (* RIGHT TAPERED WALL - P12)

N18 G02 X70.0 Z-31.687 R0.75                    (* RIGHT GROOVE RADIUS - P11)

N19 G01 Z-32.313                                          (SWEEP BOTTOM FLAT - P1)

N20 G00 X82.0 Z-32.0                                   (RETURN TO ORIGINAL START POINT)

N21 X200.0 Z100.0 T0600                             (TOOL CHANGE POSITION)

N22 M01

A few observations about the program - the middle of the groove is dimensioned as 30 mm from the front face (Z0). The selected insert is 4 mm wide. In order to position the insert exactly in the middle of the groove, the insert command point will be 2 mm further, at Z-32.0 (block N4). When the insert plunges into the material, it leaves a very small amount of stock (0.1 mm per side) at the groove bottom (block N6). The approach for the corner break is straight in the X-axis. Another option is to make this approach tangential, but that would involve another set of calculations that may be difficult to justify. Note the feedrate change for the corner breaks (blocks N10 and N16). The smaller the corner break, the slower the cutting feedrate should be - otherwise, there may not be a corner break at all or it may have a poor surface quality. The corner break method of programming described in this section can also be used for programming pulley grooves (corner breaks), described in the next section.

In this program, all Z-motions are in absolute mode. Note the blocks N14, N16, N17, and N18 (marked with an asterisk in the comment section). Each absolute Z-position has been increased by 4 mm, to compensate for the fact that it is the right corner of the insert that does the cutting. Grooves that are programmed symmetrically on both sides of their centerline may benefit from programming the Z-motions in incremental mode, to avoid this adjustment. In incremental mode, the same numbers will appear for both walls in the program, albeit with opposite signs.