Parámetros de corte recomendados para el acero para herramientas D2
Selecting appropriate machining parameters is essential when working with D2 tool steel because its high carbide content increases cutting forces and accelerates tool wear. Improper machining conditions can lead to rapid tool failure, unstable cutting behavior, and surface damage to the workpiece.
Este artículo forma parte de la Guía de mecanizado de acero para herramientas D2, which examines common manufacturing challenges encountered when machining D2 tool steel components. Equivalent grades include 1.2379 and SKD11, and the machining principles discussed here generally apply to these grades as well.
The following sections summarize recommended machining parameters for turning and grinding operations, with notes regarding milling and drilling where applicable.
Factors That Influence the Machining of D2 Tool Steel
The machinability of D2 tool steel is strongly influenced by its microstructure, which contains a high volume of hard chromium-rich primary carbides (M7C3). These carbides improve wear resistance in service but accelerate abrasive wear on cutting tools during machining.
The heat treatment condition of the steel also significantly affects machining behavior. D2 is typically machined in the fully annealed condition, where spheroidized carbides are distributed within a ferritic matrix. In this condition, cutting forces remain relatively moderate, and conventional carbide tools can be used.
When machining hardened D2 (approximately 58–62 HRC), cutting forces increase substantially, and tool wear accelerates. Hard turning operations, therefore, require specialized cutting tool materials such as PCBN or ceramic tools, along with rigid machine setups and controlled cutting conditions.
D2 Turning Parameters
For standard turning operations, D2 belongs to the group of cold-work tool steels with relatively low machinability. Recommended turning parameters depend primarily on the cutting tool material and the operation type, such as roughing, semi-roughing, or finishing.
The following ranges apply to conventional turning of D2 tool steel in the annealed condition (approximately 200–250 HB).
Table 1: Turning Parameters for D2 Tool Steel Using Coated Carbide Tools
| Operation | Depth of Cut (in.) | Feed Rate (ipr) | Cutting Speed (sfm) | Coated Carbide Grade / ISO |
| Roughing | 0.300 | 0.015 | 200 | C6 / M30, P30 |
| Semiroughing | 0.150 | 0.010 | 275 | C6 / M20, P20 |
| Finishing | 0.040 | 0.005 | 575 | C7 / M10, P10 |
Table 2: Turning Parameters for D2 Tool Steel Using Cermet Tools
| Operation | Depth of Cut (in.) | Feed Rate (ipr) | Cutting Speed (sfm) | Tool Material |
| Roughing | 0.300 | 0.015 | 550 | HPC Cermet |
| Semiroughing | 0.150 | 0.010 | 750 | HPC Cermet |
| Finishing | 0.040 | 0.005 | 1300 | HPC Cermet |
Hard Turning D2 Tool Steel
When turning D2 in the hardened condition (approximately 58–62 HRC), conventional carbide tools typically exhibit insufficient wear resistance. Hard turning operations, therefore, usually employ polycrystalline cubic boron nitride (PCBN) cutting tools.
Experimental studies have reported feasible hard turning parameters within the following ranges:
- Cutting speed: 70–120 m/min
- Feed rate: 0.08–0.20 mm/rev
Additional studies have demonstrated that hardened D2 around 58 HRC can achieve surface roughness values between Ra 0.28 and 1.12 µm using cutting speeds between 80 and 220 m/min, feed rates between 0.05 and 0.15 mm/rev, and a depth of cut of approximately 0.2 mm.
D2 Milling Parameters
Available sources describe high-speed end milling of hardened D2 tool steel using various cutting tool materials such as coated carbide, cermet, PCBN, and solid carbide tools. These studies primarily evaluate tool wear behavior and achievable surface finish rather than providing generalized parameter tables.
Because milling parameters vary significantly depending on cutter diameter, tool geometry, coating type, machine rigidity, and whether the material is annealed or hardened, the consulted sources do not provide standardized tables specifying cutting speed, feed rate, or depth of cut for milling operations.
As a result, no generalized milling parameter tables for D2 tool steel are available in the literature.
D2 Drilling Parameters
The consulted sources provide drilling calculations and parameter tables for general carbon steels and alloy steels, but they do not include specific drilling data for D2 tool steel.
Drilling operations in D2 are typically performed in the annealed condition, as the material becomes significantly more difficult to machine after hardening. Tool material selection, coolant application, and machine rigidity, therefore, strongly influence drilling performance.
Because the available references do not provide verified cutting speed or feed recommendations specifically for drilling D2 tool steel, no drilling parameter tables are included in this guide.
D2 Grinding Recommendations
Due to its high abrasion resistance and large volume of primary carbides, D2 tool steel is susceptible to thermal damage during grinding. Excessive stock removal or insufficient coolant can generate localized overheating, which may cause over-tempering of the surface, formation of a brittle rehardened “white layer,” or grinding cracks.
The following table summarizes recommended parameters for surface grinding D2 tool steel using conventional grinding wheels.
Table 3: Surface Grinding Parameters for D2 Tool Steel (Conventional Wheels)
| Condition / Hardness | Wheel Speed (fpm) | Table Speed (fpm) | Downfeed (in/pass) | Crossfeed (in/pass) | Wheel Identification |
| Annealed (Max 50 HRC) | 5500 – 6500 | 50 – 100 | Rough: 0.003Finish: 0.0005 max | 0.050 – 0.500 | A46JV |
| Hardened (50–58 HRC) | 3000 – 4000 | 50 – 100 | Rough: 0.002Finish: 0.0005 max | 0.025 – 0.250 | A46IV |
If CBN grinding wheels are used for surface grinding annealed D2 (maximum 50 HRC), wet wheel speeds can be increased to 5500–8000 fpm when using a B100T75B wheel.
For cylindrical grinding of annealed D2, an A60KV wheel is recommended with wheel speeds of 5500–6500 fpm and work speeds of 60–100 fpm.
General Machining Guidelines for D2 Tool Steel
Machine Rigidity
Machining D2 generates relatively high cutting forces due to the presence of hard primary carbides. Machine tools must therefore provide sufficient stiffness and damping capacity, and tool overhang should be minimized to reduce vibration and chatter.
Shaping Adjustments
When shaping Acero para herramientas D2 compared with lower-alloy tool steels such as W2, cutting speeds are typically reduced by approximately 30% and feed rates by about 50% to account for D2’s lower machinability. Typical ram speeds for shaping operations are around 12.5 m/min (41 sfm) with a feed of 0.25 mm (0.010 in.) per stroke.
Post-Grinding Stress Relief
Grinding operations can introduce residual stresses and may locally transform surface microstructures. For critical tooling components, it is recommended to apply a stress-relieving temper after grinding.
This tempering operation is typically performed at approximately 40 °C (80 °F) below the original tempering temperature, allowing the surface to regain toughness without significantly reducing the tool’s final hardness.
Páginas relacionadas
- ¿Por qué es difícil mecanizar el acero para herramientas D2?
- ¿Por qué se producen grietas por rectificado en el acero para herramientas D2?
- ¿Por qué se agrieta el acero para herramientas D2 durante el mecanizado por electroerosión?
Preguntas frecuentes
For roughing, use 200 sfm with a 0.015 ipr feed. Semi-roughing requires 275 sfm and 0.010 ipr, while finishing uses 575 sfm and 0.005 ipr.
Roughing operations use 550 sfm, semi-roughing uses 750 sfm, and finishing reaches 1300 sfm. Feeds range from 0.015 ipr for roughing to 0.005 ipr for finishing.
Hard turning (58–62 HRC) using PCBN tools typically requires speeds of 70–120 m/min. Feeds should range between 0.08 and 0.20 mm/rev to maintain stability.
Annealed D2 uses 5500–6500 fpm wheel speeds, while hardened D2 (50–58 HRC) requires 3000–4000 fpm. Both conditions use a table speed of 50–100 fpm.
Use an A60KV wheel with wheel speeds of 5500–6500 fpm. Work speeds should be maintained between 60 and 100 fpm for annealed material.
Compared to W2, reduce cutting speeds by 30% and feed rates by 50%. Typical ram speeds are 12.5 m/min with a feed of 0.25 mm per stroke.
For surface grinding annealed D2 with a B100T75B wheel, wet wheel speeds can be increased to 5500–8000 fpm. This offers a higher speed range than conventional wheels.