During CNC programming, the programmer must determine the cutting parameters for each operation and incorporate them into the program in the form of instructions. These cutting parameters include cutting speed, depth of cut, and feed rate, among others. Different machining methods require the selection of specific cutting parameters tailored to each process.
1. Principles for Selecting Cutting Parameters
During rough machining, the primary objective is generally to maximize productivity; however, economic efficiency and machining costs must also be taken into consideration. For semi-finish and finish machining, the focus shifts to balancing cutting efficiency, economic viability, and machining costs while simultaneously ensuring the required machining quality. The specific numerical values for these parameters should be determined based on the machine tool's technical specifications and cutting parameter handbooks, supplemented by practical experience.
From the perspective of tool life and durability, the recommended sequence for selecting cutting parameters is as follows: first determine the depth of cut, followed by the feed rate, and finally, the cutting speed.
2. Determining the Depth of Cut
The depth of cut is determined by the rigidity of the machine tool, the workpiece, and the cutting tool. Provided that the rigidity of the system permits it, the depth of cut should ideally be set equal to the total machining allowance (stock removal) of the workpiece; this approach minimizes the number of passes required, thereby enhancing production efficiency.
Principles for determining the depth of cut:
(1) When the required surface roughness of the workpiece falls within the range of Ra 12.5 μm to 25 μm, and the machining allowance is less than 5 mm to 6 mm, the rough machining process can typically be completed in a single pass to meet the specifications. However, if the machining allowance is substantial, the rigidity of the process system is insufficient, or the machine tool lacks adequate power, the operation may be divided into multiple passes.
(2) When the required surface roughness falls within the range of Ra 3.2 μm to 12.5 μm, the process should be divided into two stages: rough machining and semi-finish machining. The selection of the depth of cut for the rough machining stage follows the principles outlined above. After rough machining, a residual allowance of 0.5 mm to 1.0 mm should be left on the workpiece surface, to be subsequently removed during the semi-finish machining stage.
(3) When the required surface roughness falls within the range of Ra 0.8 μm to 3.2 μm, the process should be divided into three stages: rough machining, semi-finish machining, and finish machining. For the semi-finish machining stage, the depth of cut should be set between 1.5 mm and 2 mm. During finishing operations, the depth of cut should be set between 0.3 mm and 0.5 mm.
3. Determining the Feed Rate
The feed rate is primarily selected based on the required machining precision and surface roughness of the part, as well as the materials of the cutting tool and the workpiece. The maximum feed rate is limited by the rigidity of the machine tool and the performance capabilities of its feed system.
Principles for Determining the Feed Rate:
1) When the quality requirements of the workpiece can be guaranteed, a higher feed rate may be selected to enhance production efficiency. Generally, a value within the range of 100 to 200 m/min is chosen.
2) When performing cutoff operations, machining deep holes, or utilizing high-speed steel tools, it is advisable to select a lower feed rate; typically, a value within the range of 20 to 50 m/min is chosen.
3) When high demands are placed on machining precision and surface roughness, a lower feed rate should be selected; generally, a value within the range of 20 to 50 m/min is chosen.
4) During non-cutting tool movements-particularly when returning to the "zero point" over a long distance-the maximum feed rate configured within the machine tool's CNC system may be selected.
4. Determining the Spindle Speed
The spindle speed should be selected based on the permissible cutting speed and the diameter of the workpiece (or the cutting tool). The calculation formula is as follows:
n = 1000v / πD
v - Cutting speed (in m/min), determined by the durability of the cutting tool;
n - Spindle speed (in r/min);
D - Diameter of the workpiece or cutting tool (in mm).
The calculated spindle speed *n* must ultimately be adjusted to match one of the available speeds listed in the machine tool's specifications, or the closest available speed. In summary, the specific values for cutting parameters should be determined based on the machine tool's performance capabilities and relevant technical manuals, combined with practical experience, often utilizing an analogical approach. Furthermore, the spindle speed, depth of cut, and feed rate should be harmonized to ensure mutual compatibility, thereby establishing the optimal set of cutting parameters.
Reference Formula:
(I) Depth of Cut (ap): The perpendicular distance between the machined surface of the workpiece and the surface yet to be machined is defined as the depth of cut. The *depth of cut* ($a_p$) is the amount of material removed, measured from a reference point on the cutting edge in a direction perpendicular to the working plane. It represents the depth to which the turning tool penetrates the workpiece during each feed pass; hence, it is also referred to as the *cutting depth*. Based on this definition, when performing longitudinal turning on an external cylindrical surface, the depth of cut can be calculated using the following formula:
$a_p = (d_w - d_m) / 2$
Where: $a_p$ - depth of cut (mm); $d_w$ - diameter of the workpiece surface *prior* to machining (mm);
$d_m$ - diameter of the workpiece surface *after* machining (mm).
**Example 1:** Given a workpiece with an initial surface diameter of $\Phi 95$ mm, if it is turned in a single pass to a diameter of $\Phi 90$ mm, calculate the depth of cut.
**Solution:** $a_p = (d_w - d_m) / 2 = (95 - 90) / 2 = 2.5$ mm.
**(II) Feed Rate ($f$)**
This refers to the relative displacement between the cutting tool and the workpiece-measured in the direction of the feed motion-for every full revolution of the workpiece or tool. Depending on the direction of the feed, it is classified into *longitudinal feed* and *transverse feed*. Longitudinal feed refers to the feed motion directed along the guide rails of the lathe bed, while transverse feed refers to the feed motion directed perpendicular to the guide rails of the lathe bed. (Note: *Feed velocity* ($v_f$) refers to the instantaneous velocity of a selected point on the cutting edge relative to the workpiece during the feed motion.)
$v_f = f \cdot n$
Where: $v_f$ - feed velocity (mm/s);
$n$ - spindle speed (r/s);
$f$ - feed rate (mm/rev).
**(III) Cutting Speed ($v_c$)**
This refers to the instantaneous velocity of a selected point on the cutting edge relative to the workpiece during the *primary motion* (rotation). The calculation formula is as follows:
$v_c = (\pi \cdot d_w \cdot n) / 1000$
Where: $v_c$ - cutting speed (m/min);
$d_w$ - diameter of the workpiece surface *prior* to machining (mm);
$n$ - workpiece rotational speed (r/min). When performing calculations, the maximum cutting speed should be used as the reference point; for instance, during turning operations, calculations should be based on the diameter of the surface being machined, as this is where the velocity is highest and tool wear occurs most rapidly. Example 2: Turning the outer diameter of a workpiece with a diameter of Φ60 mm. The selected lathe spindle speed is 600 r/min. Calculate *v*c. Solution: *v*c = (π * d*w * n) / 1000 = 3.14 × 60 × 600 / 1000 = 113 m/min. In actual production, the workpiece diameter is typically a known quantity. Based on factors such as the workpiece material, tool material, and machining requirements, a specific cutting speed is selected; this cutting speed is then converted into the corresponding lathe spindle speed to facilitate the proper adjustment of the machine tool. This conversion yields the following formula: n = (1000 * *v*c) / (π * d*w). Example 3: Turning the outer diameter of a Φ260 mm pulley on a CA6140 horizontal lathe. A cutting speed (*v*c) of 90 m/min is selected. Calculate *n*. Solution: n = (1000 * *v*c) / (π * d*w) = (1000 × 90) / (3.14 × 260) = 110 r/min. Once the lathe spindle speed has been calculated, one should select a value from the machine's nameplate that is closest to the calculated result; in this instance, n = 100 r/min is selected as the actual operating speed for the lathe. III. Summary: Cutting Parameters 1. Depth of Cut (*a*p) (mm): *a*p = (*d*w - *d*m) / 2 (mm) 2. Feed Rate (*f*) (mm/rev) 3. Cutting Speed (*v*c) (m/min): *v*c = π * d * n / 1000 (m/min); n = 1000 * *v*c / (π * d) (r/min)
