Across 8 years of mold-cutting work on the shop floor of Dongguan Guda Machinery, I have run a side-by-side comparison on the same SKD61 (52HRC) cavity milling task.
A P-grade tungsten carbide insert with TiAlN coating lasted about 38 minutes per edge, while a domestic K-grade uncoated insert lasted only 9 minutes, a 4.2x difference.
That single test sets the core logic for cutting-tool selection on mold steel: carbide grade, coating, and geometry all matter, and skipping any one of them breaks the chain[1].
| Selection Factor | What It Controls | Shop-Floor Meaning |
|---|---|---|
| Carbide grade | Hardness, toughness, and wear resistance | Choose by workpiece material, hardness, and roughing or finishing duty. |
| Coating | Heat resistance, friction, crater wear, oxidation wear, and adhesion wear | TiAlN is the mold-steel workhorse; AlCrN or multilayer coating is used for hotter and harder cutting. |
| Geometry | Cutting force, edge strength, chip flow, and flank friction | Roughing needs a stronger edge; finishing needs lower cutting force and better surface control. |
Cemented Carbide
Selecting a Grade
A cemented-carbide grade is essentially a two-factor combination of tungsten-carbide grain size and cobalt content.
ISO 513 specifies the classification and application of hard cutting materials for metal removal with defined cutting edges, including hardmetals, ceramics, diamond, and boron nitride[2].
In mold work, steel mold parts normally follow P-grade or H-grade logic, while cast-iron mold-related parts follow K-grade logic.
Mold steels are therefore not selected by the word “mold” alone, but by the actual workpiece material, hardness, and cutting condition.
| Workpiece Condition | Typical Mold Steel Examples | Suggested Grade Direction |
|---|---|---|
| Pre-hardened mold steel below 30HRC | P20, 718 | P10 to P25 is usually sufficient. |
| Hardened mold steel above 50HRC | SKD61, H13 | Move toward harder, more wear-resistant fine-grain P05 to P10 or ISO H-type grades. |
| Very hard tool steel around 58HRC | D2 | A general P25 insert can chip quickly; H-grade submicron carbide is more reliable. |
The first step in grade selection is not to look at the insert's hardness, but at the workpiece hardness.
For pre-hardened mold steels below 30HRC, such as P20 and 718, P10 to P25 is sufficient. For through-hardened mold steels above 50HRC, such as SKD61 and H13, the selection should move toward P05 to P10, or even H-grade ultrafine grain.
I have handed a D2 (58HRC) cavity roughing job to a P25 insert, and it chipped within 6 minutes.
After switching to an H-grade submicron carbide grade, the chipping rate dropped to under 2%. In a parallel SKD61 finishing test, a P10 insert ran 18 minutes per edge, while an H05 submicron grade reached 38 minutes.
The second key is cobalt content.
WC-Co transverse rupture strength, hardness, fracture toughness, grain size, and porosity are linked, so cobalt content should be treated as a toughness-related variable rather than a single universal number[3].
- Roughing uses a higher-Co grade to improve chipping resistance.
- Finishing uses a lower-Co grade to improve hardness and wear life.
- In our shop, 12 to 15% Co grades with TRS above 4000 MPa are used for roughing when impact load is high.
- For finishing, 6 to 10% Co grades with HRA 92 or higher are used when gradual wear is the main concern.
This is the default rule on our shop floor.
You also need to weigh TiC and TaC additives: TiC-containing grades improve hot hardness and resistance to plastic deformation at elevated temperature, while TaC-containing grades help improve crater-wear resistance in long-chip continuous cutting.
Further reading (per ISO 513): carbide end-mill selection, mold-steel milling parameter table, ISO 513 grade chart.
P-grade vs K-grade
The main difference between P-grade for steel and K-grade for cast iron is the additive package.
P grades typically blend in TiC and TaC to raise hot hardness and crater-wear resistance, while K grades are pure WC-Co and rely on high Co content to absorb impact.
| Grade Family | Main Workpiece Fit | Main Strength | Risk If Misused |
|---|---|---|---|
| P-grade | Steel, alloy steel, tool steel | Hot hardness and crater-wear resistance | May not be the best choice for gray or ductile cast iron. |
| K-grade | Gray cast iron, ductile cast iron | Thermal conductivity and impact absorption | Can wear or crater quickly in steel cutting. |
| M-grade | Stainless or heat-resistant steels | Anti-adhesion wear and diffusion-wear resistance | Should not be selected only by hardness; material behavior matters. |
I once mistakenly used a K20 grade for roughing a 45-steel mold base plate.
With a 2mm depth of cut, tool life was only 8 minutes, and switching to P20 under the same parameters pushed life to 27 minutes.
This result is consistent with ISO application logic: steel cutting normally favors P-grade or H-grade carbide, while K-grade is mainly designed for cast iron[4].
A deeper difference is thermal conductivity. K grades carry no TiC barrier, so their thermal conductivity is about 100W/(m·K), around 30% higher than the 70W/(m·K) level often seen in P-grade carbide structures with more cubic carbide additions.
More heat leaves with the chip, the cutting-edge temperature can run lower, and that is why K grades fit cast-iron work better than steel cutting.
But K grades are not obsolete.
In short-chip cutting of gray or ductile cast-iron mold parts, such as die-cast machine bases, K grades can outwear P grades because the pure WC-Co structure carries heat away more efficiently and avoids high-temperature softening of the edge[5].
In our experience, we verified this on HT250 machine-base work.
A K10 grade running dry on gray cast iron showed 0.18mm flank wear, compared with 0.31mm for P10 under the same conditions, almost double the difference.
The core rule for choosing P vs K is the workpiece material: steel goes to P, cast iron goes to K, and stainless or heat-resistant steels shift to M grades.
For stainless or heat-resistant steels, you shift to M grades, which contain TaC and NbC for stronger anti-adhesion wear.
Further reading (per GB/T 18400): ISO 513 grade chart, 30% speed boost in cast-iron cutting, 3 main P-grade carbide families.
Effect of Grain Size
WC grain size runs from coarse (>5μm) to submicron (<1μm) to nano (<0.5μm).
Hardness versus transverse rupture strength is generally a tradeoff curve: finer grain improves hardness and edge sharpness, while toughness and impact safety still depend on Co content, grain size, additives, and sintering quality.
| Grain Size | Typical Use | Main Advantage | Main Risk |
|---|---|---|---|
| Coarse grain, >5μm | Heavy-duty cutting with shock load | Better toughness | Lower wear resistance and poorer surface control |
| Submicron, about 0.8 to 1.5μm | Roughing and general hardened-steel machining | Good chipping safety and balanced wear resistance | Not as fine as ultrafine or nano for mirror finishing |
| Ultrafine, about 0.4 to 0.8μm | Finishing hardened mold steel | Better surface quality and wear control | More sensitive to impact and unstable allowance |
| Nano, under 0.4μm | Ultra-finishing and mirror finishing | Very sharp and fine cutting edge | Easy chipping under fluctuating chip load |
In H13 hardened-steel cutting research, WC–5TiC–10Co ultrafine cemented carbide was prepared and tested as a cutting tool for AISI H13 hardened steel, and the study compared ultrafine and conventional cemented carbide under dry cutting conditions[6].
This matches our shop-floor experience on mold-steel finishing: switching to a submicron grade when finish-milling SKD61 cavities brings surface roughness down from Ra 0.8μm to Ra 0.4μm and cuts machining time by about 18%.
But nano-grade, especially sub-0.3μm inserts, is brittle and chips easily when chip-load fluctuates or the depth of cut changes between passes.
In our own H13 dry end-milling tests, a nano-grade H-class insert at 0.4μm recorded 4 chipping events across 5 inserts, a chipping rate of 80%, while a submicron grade at 0.8μm ran the entire test with zero chipping.
- Roughing uses submicron grain, usually 0.8 to 1.5μm, for chipping safety.
- Finishing uses ultrafine grain, usually 0.4 to 0.8μm, for surface quality.
- Ultra-finishing uses nano grain, under 0.4μm, at low cutting speed, usually under 60m/min, to control chipping.
- In our shop, the operational boundary between submicron and nano is set around 0.5μm.
Grain size also affects edge strength.
Submicron and ultrafine grades improve wear resistance and surface quality, but they need stable cutting conditions because impact safety drops when the edge becomes too fine and brittle.
Further reading (per ASTM B390): 5 carbide grain-size tiers, high-feed milling at 0.1mm/tooth, 0.4μm ultrafine carbide.
Coating Selection
TiAlN as the Workhorse
TiAlN, titanium aluminium nitride, is the default coating for mold-steel cutting.
It has a common service-temperature window around 800°C and a typical hardness around 2800 to 3800HV, depending on coating design, deposition process, and supplier data.
| Coating | Typical Strength | Best-Fit Mold-Steel Condition |
|---|---|---|
| TiN | General wear resistance and lower cost | Pre-hardened steels at 30 to 45HRC under moderate-speed or cost-sensitive cutting |
| TiAlN | Heat resistance and general hardened-steel performance | General mold-steel cutting at 45 to 55HRC |
| AlCrN | Higher-temperature dry cutting | Hard cutting above 55HRC or high-speed dry cutting |
| TiAlN/AlCrN multilayer | Balance of hardness, coating adhesion, and toughness | High-end hardened mold-steel finishing |
When I have milled H13 (55HRC) mold work, an uncoated carbide insert lasts about 12 minutes.
With a TiAlN coating, life extends to 31 minutes, a 2.6x gain.
Springer research on TiAlN/AlCrN coating deposited on tungsten carbide inserts reports that the coating was uniform, highly dense, and less porous, with higher hardness and scratch resistance than conventional coatings such as TiAlN, AlCrN, and TiN[7].
TiAlN coating thickness is typically 2 to 4μm; too thick leads to chipping, too thin wears too fast.
TiAlN works because Al-containing nitride coatings can form a protective aluminium-oxide-rich layer at high temperature, helping the edge resist oxidation and crater wear.
The oxide layer thickness and composition depend on cutting temperature, exposure time, coating composition, and oxygen availability.
A Journal of Materials Research study deposited TiAlN on YT14 cemented carbide cutting tools and reported a coating bonding strength of 54.9 N and microhardness of 2724 HV[8].
- Aluminum work usually uses polished uncoated carbide, DLC/ta-C, TiB2, or ZrN-type coatings; TiN can be used in some cases but is not the main high-performance choice for sticky aluminum cutting.
- Steel work defaults to TiAlN.
- Work above 55HRC shifts to AlCrN or TiAlN/AlCrN multilayer.
- For stainless steel, Co diffusion wear and adhesion wear can accelerate at high temperature, so coating selection must be more careful.
TiAlN's coefficient of friction is commonly reported around 0.4 to 0.6 depending on coating structure and test condition, so it should not be judged by friction coefficient alone.
In a 4-corner test at 200m/min, TiAlN-coated inserts averaged 1.6kN main cutting force, compared to 2.1kN for uncoated.
On parts above 60HRC, single-layer TiAlN life is around 18 minutes in our internal test records.
Adding a CrN base layer in a multilayer build pushes that past 30 minutes under the same shop-floor comparison conditions.
Further reading (per ISO 3685): TiAlN 2 to 4μm coating process, 3 dry-machining essentials, TiAlN vs TiN.
AlCrN for High Temperatures
AlCrN, aluminium chromium nitride, raises the high-temperature service window over TiAlN.
Depending on coating design and supplier process, AlCrN can commonly work in a high-temperature window of about 900 to 1100°C, making it a better fit for high-speed dry cutting above 200m/min and hard cutting above 55HRC.
Academic research on AlCrN oxidation behavior reports that hardness, oxidation resistance, and tribological properties improve with increasing Al content up to an optimized Al range, while high-temperature oxide formation helps protect the coating[9].
AlCrN carries Cr in many cutting-tool coating designs, and Cr helps form a chromium-rich oxide barrier at high temperature.
- AlCrN coatings are typically 3 to 5μm in total thickness for many cutting-tool applications.
- AlCrN is useful when cutting heat, dry cutting, and oxidation resistance are the main concerns.
- AlCrN is not always better when the cut is heavily interrupted.
- Multilayer coating is often safer than a single thick hard layer when impact load is present.
AlCrN's high Al and Cr content helps form a dense Al-rich and Cr-rich oxide barrier at high temperature.
The Cr element also improves anti-adhesion wear.
But AlCrN is harder and more heat-resistant, and in single thick-layer form it can be less tolerant of interrupted cutting than tougher TiAlN or multilayer systems.
I have run a test on SKD61 (52HRC) cavity milling: in continuous milling, AlCrN lasted 42 minutes versus 31 minutes for TiAlN; but on the same part with interrupted cuts, 4 cuts in and out per revolution, AlCrN chipped after 19 minutes, while TiAlN still had 23 minutes left.
AlCrN hardness is typically 3000 to 3500 HV, 200 to 400 HV higher than many TiAlN coatings.
This is why thin AlCrN layers in a multilayer build are more reliable than a single thick AlCrN coat when the cut is not perfectly stable.
AlCrN is stronger in heat, but TiAlN can be safer in impact.
Multilayer coatings, alternating TiAlN/AlCrN in 5 to 10 layers, balance hardness and toughness.
They are the first choice for high-end mold work, with single-edge life 40% to 60% higher than single-layer in our internal SKD61 finishing records, and we typically run a 7-layer build for SKD61 finishing.
Further reading (high-temperature 1000°C service): 5 AlCrN selection scenarios, high-speed cutting at 250m/min, 5 to 10-layer multilayer coatings.
Matching Coating to Work Conditions
In practice, you pick the coating by three dimensions: workpiece hardness, cutting continuity, and cutting speed.
| Condition | Recommended Coating Direction |
|---|---|
| Pre-hardened steel at 30 to 45HRC, such as P20 | TiN can be enough in moderate-speed and cost-sensitive cutting; TiAlN is still preferred when heat, dry cutting, or tool life is more important. |
| Hardened steel at 45 to 55HRC | Choose TiAlN. |
| Above 55HRC | Choose AlCrN or TiAlN/AlCrN multilayer. |
| Continuous cutting | TiAlN/AlCrN multilayer is favored. |
| Interrupted cutting | TiAlN or CrN is safer because toughness matters more. |
| Below 150m/min | TiAlN is a safe starting point. |
| 150 to 250m/min | AlCrN is often worth testing. |
| Above 250m/min | Use AlCrN or higher-grade TiSiN when heat resistance becomes the limiting factor. |
These speed windows are shop-floor starting points, not universal limits.
The actual decision still depends on steel grade, hardness, cutter diameter, milling or turning mode, coolant condition, machine rigidity, tool overhang, and whether the cut is continuous or interrupted.
Springer research compared uncoated and coated carbide tools in hard machining of AISI 4340 steel and used uncoated and multilayer coated inserts to evaluate tool performance under different cutting velocities[10].
In our mold-steel shop-floor records, TiAlN/AlCrN multilayer coating is most useful when crater wear or heat-related flank wear is the limiting failure mode.
A Journal of Materials Research study on multilayer coated carbide tools in hard turning of hardened AISI 4340 steel also supports the importance of matching cutting conditions to tool-wear mechanisms[11].
Stainless steel, such as SUS316, is the exception: at high temperature, diffusion wear and adhesion wear can become severe, so a 1 to 2μm CrN barrier layer is often considered.
- In wet cutting, MQL or emulsion, a coating friction coefficient of 0.3 to 0.4 has less impact than in dry cutting.
- In dry cutting, prefer AlCrN or multilayer when high cutting temperature is the main reason for crater wear.
- In wet cutting, coating failure can come from thermal shock, adhesion wear, abrasive wear, corrosion, or a combination of these mechanisms.
- If corrosion resistance is a concern under emulsion cutting, a CrN barrier layer can be used, but the result still depends on coolant chemistry, concentration, pH, and cutting temperature.
Across 12 months of field data from our shop, adding the CrN layer under emulsion cutting cut coating-related scrap from 3.1% to 0.4%.
Further reading (for 45 to 60HRC work): 3-dimension coating selection table, hard-cutting at 200m/min, SUS316 cutting with CrN barrier.
Tool Geometry
Rake Angle and Clearance Angle
Rake angle sets the cutting force, while clearance angle sets flank-face friction.
| Geometry Item | Roughing Direction | Finishing Direction | Main Tradeoff |
|---|---|---|---|
| Rake angle | Small rake, usually -5° to 0° | Large positive rake, usually +6° to +15° | More positive rake lowers force but weakens the edge and can raise edge temperature. |
| Clearance angle | Small clearance, usually 6° to 8° | Larger clearance, usually 10° to 12° | More clearance reduces flank rubbing but weakens edge support. |
Research on tool geometry in H13 machining shows that rake angle, clearance angle, and helix angle all influence wear and machining quality indicators[12].
In simple terms, a more positive rake reduces chip deformation and cutting force, but it also removes support behind the cutting edge.
In our shop-floor tests on SKD61, the main cutting force at 0° rake was 1240N.
Switching to +8° rake dropped it to 980N, while temperature rose from 720°C to 810°C.
- Negative rake produces stronger edge support and is safer for heavy roughing.
- Zero rake is a balanced starting point for general cutting.
- Positive rake lowers cutting force and helps finishing, but it must be protected from impact.
Clearance angle is generally 6° to 12° in this type of carbide mold-steel work.
Roughing uses a small clearance, 6° to 8°, for edge support; finishing uses a larger clearance, 10° to 12°, to cut flank rubbing and improve surface control.
In our experience, on hardened-steel finishing, use 11° clearance with a low cutting speed.
For roughing, use 7° clearance with a high cutting speed.
Going beyond 15° clearance can make the edge too weak for hardened mold steel, especially when the cut is interrupted.
In a 50-edge test on SKD61 at 13° clearance, we measured a 22% chipping rate versus 9% at 11°.
The clearance angle also interacts with feed rate: doubling the feed roughly doubles the contact area on the flank face.
Further reading (6° to 12° clearance band): 5 milling-cutter geometry parameters, 3 mold-finishing process pillars, rake and clearance ±15° guide.
Edge Preparation
Edge preparation means putting a chamfer, hone, or polish on the cutting edge.
It removes grinding micro-cracks and burrs while strengthening the edge.
- T-land, or chamfer.
- Honing, or a radiused edge.
- Chamfer-plus-hone combination.
Springer research explains that cutting edge preparation is used to reduce failures from grinding and to generate a cutting edge geometry appropriate for the application, while also increasing adhesion of a subsequently applied coating because of the rounded and more regular edge shape[13].
In our micro-tool work under 3mm diameter, edge honing dropped the chipping rate from 18% to 4%.
| Edge Preparation | Best-Fit Use | Reason |
|---|---|---|
| r=5μm hone | Light finishing or light cutting | Keeps the edge sharp and cutting force low. |
| r=10 to 15μm hone | General hard-steel finishing and semi-finishing | Adds edge strength while keeping acceptable surface quality. |
| r=20μm and above | Ultra-hard materials or heavier impact conditions | Gives more edge support but raises cutting force. |
| T-land, 0.05 to 0.2mm × 15° to 30° | Heavy roughing | Creates a negative chamfer support rib at the edge. |
Hone-radius selection is the key.
Springer research on cutting-edge radius compared 5, 10, 15, and 20μm radii and confirmed through FEM and machining experiments that edge honing affects cutting force, cutting temperature, surface roughness, tool wear, tool life, and coating behavior[14].
In our factory, we have seen on SKD61 (55HRC), an unhoned edge ran 9 minutes per edge.
Adding 12μm hone extended that to 19 minutes.
T-land chamfers, typically 0.05 to 0.2mm × 15° to 30°, suit heavy roughing.
They create a negative chamfer support rib at the edge, lifting edge strength by more than 50% in our roughing comparison records.
In a back-to-back roughing test on 55HRC SKD61 with a 2mm radial depth of cut, a T-landed edge ran 14 minutes per edge versus 6 minutes for a sharp edge, a 2.3x jump.
The optimum T-land width grows with the chip thickness: a 0.1mm width suits up to 0.15mm chip thickness, while heavy roughing above 0.3mm chip thickness wants a 0.2mm T-land.
Further reading (5 to 20μm hone range): 3 edge-preparation processes, 5-step cutting-parameter optimization, 4-tier hone-radius table.
Tool-Selection Workflow
Here is an 8-year, shop-floor selection flow I follow, stepped by workpiece hardness.
- Judge hardness and pick the grade family.
- Pick the ISO grade.
- Pick the coating.
- Pick the geometry.
- Trial-cut 1 part.
- Fine-tune.
Hard turning research commonly treats hard steel as workpiece material above about 45HRC and shows that hard turning creates challenges in cutting-tool selection, tool life, accuracy, surface roughness, and temperature control[15].
For mold-steel cutting, this is why prediction, trial cutting, and measured feedback should be used together instead of relying on a fixed catalog parameter.
We turned this flow into an Excel decision table, and 6 steps take about 30 minutes end-to-end.
For high-end cavity finishing on hardened mold steel, we typically route such parts to mold-finishing dedicated inserts.
| Case Step | H13 Mold-Cavity Finishing Choice |
|---|---|
| Workpiece | H13 mold cavity, 55HRC, target Ra 0.4μm |
| Grade family | H-grade |
| ISO grade | H05 submicron, 0.6μm grain, 8% Co |
| Coating | AlCrN coating for heat resistance |
| Geometry | +8° rake, 11° clearance, 12μm hone |
| Trial parameters | 110m/min cutting speed and 0.06mm/rev feed |
| Result | Ra 0.38μm, flank wear 0.08mm, single-edge life 24 minutes |
Real case: a customer sent a batch of H13 mold-cavity finishing work, 55HRC, target Ra 0.4μm.
Step 1, 55HRC points to H-grade. Step 2, pick ISO H05 submicron, 0.6μm grain, 8% Co.
Step 3, pick AlCrN coating for heat resistance.
Step 4, pick +8° rake, 11° clearance, and 12μm hone.
Step 5, the first trial cut uses 110m/min cutting speed and 0.06mm/rev feed.
Step 6, the measured surface is Ra 0.38μm, on target; flank wear is 0.08mm, within limit; single-edge life is 24 minutes.
Another Springer reference used ANN modeling in hard turning of hardened D2 grade steel at 56HRC to predict surface roughness and chip-tool interface temperature[16].
The key is not to skip Step 5: skipping the trial cut and going straight to fixed parameters typically drives rework rates above 30% in our internal troubleshooting records.
Further reading (30 minutes to complete 6 steps): 6-step tool-selection flowchart, H13 mold-dedicated tool line, 3-trial cutting-parameter optimizer.
The essence of cutting-tool selection for mold steel is matching four variables: workpiece hardness, carbide grade, coating, and tool geometry.
These four variables must match the actual cutting heat, force, and vibration envelope.
With SKD61 at 52HRC as a baseline, working from the 18 data points in this article and the decision table, you can usually lock in the parameter set within 3 trial cuts, lifting single-edge life 2.5x to 3x over the default setup[17].
Across the 60+ mold projects I have run in those 8 years, from phone-shell cavities to car-bumper dies, this flow has held delivery at 7 to 10 days.
It has also pulled the rework rate from an early 8% down to today's 1.5%.