Can the LJ-855 Machine Pre-Hardened Mold Steel | Spindle Speed, Tooling and Finish-Pass Limits

The LJ-855 is a high-speed CNC milling machine commonly configured with a 12,000 RPM BT40/CAT40 spindle. Depending on the spindle option, rated power can reach 15 kW.^[6]

When machining pre-hardened mold steel at 28-32 HRC,^[1] three settings decide the final result: spindle speed, tooling selection, and finish-pass stock.

For P20 and P20+ grade pre-hardened mold steel, the practical finishing stock window is usually 0.3-0.5 mm. Finish-pass depth should normally stay within 0.2-0.4 mm, and 0.5 mm should be treated as the upper limit unless tool rigidity, fixture support, and spindle load are verified.

If cutting speed is too low, the insert starts rubbing instead of shearing. This can create a work-hardened surface layer, increase heat, shorten tool life, and cause dimensional drift.

Set Spindle Speed

Match Steel Hardness

Machining pre-hardened mold steel on the LJ-855 should start with checking the real hardness of the workpiece, not simply reading the material certificate.

P20 is usually around 28-30 HRC, while P20+ or similar improved grades are commonly around 30-32 HRC.

Both are called pre-hardened mold steel, but the higher-hardness material can create 15-20% higher cutting force under the same tool and speed conditions.

In small-batch production, hardness variation inside one lot can reach about 2 HRC. In 2024, I found incoming stock whose surface hardness differed from the mill certificate by more than 1.5 HRC.

· Measure three points before cutting: both ends and the center of the workpiece surface.

· Use the average value as the machining reference.

· Mark any material that is more than 1.5 HRC above the expected range.

· Reduce cutting speed or feed before the first cut when hardness is high.

The spindle speed formula is:

n = (1,000 × Vc) / (π × D)

In this formula, n is spindle speed in RPM, Vc is cutting speed in m/min, and D is cutter diameter in mm.

For pre-hardened mold steel around 30 HRC, a practical cutting speed range is 120-180 m/min. For material above 32 HRC or unstable setups, cutting speed should be reduced to about 80-120 m/min.^[8]

For every 1 HRC increase in hardness, tool life can drop by roughly 10-15% under the same cutting conditions.^[3]

The LJ-855 spindle display shows the commanded speed, not always the real cutting speed under load. If spindle load is high, actual speed can drop several percent below the panel value.

When setting speed, add a small compensation buffer only after checking spindle load and cutting sound. Do not simply increase RPM without confirming that the tool, holder, and fixture can remain stable.

Control Cutting Heat

Pre-hardened mold steel does not release cutting heat as easily as ordinary low-carbon steel. P20-type mold steel is usually around 30-40 W/(m·K), depending on grade and heat treatment, while ordinary structural steel is often higher.

This means heat tends to stay closer to the tool-chip contact zone. If the insert edge temperature becomes too high, coating wear, crater wear, and edge softening accelerate.

I have seen insert failure within the first hour during a 3-shift production run. The operator increased radial depth from 0.3 mm to 0.5 mm to save time, and tool life dropped from about 120 minutes to about 40 minutes.

The lesson is simple: in pre-hardened mold steel, a small increase in cutting depth can create a large increase in heat and tool wear.

The cooling strategy should be continuous and stable.

· For external flood cooling, keep the cutting zone fully covered and use at least 15 L/min when the machine setup allows it.

· If through-spindle coolant is available, high-pressure coolant around 80-120 bar can be used for deep cavities and difficult chip evacuation.

· Avoid intermittent cooling, because repeated heating and cooling can create thermal shock at the cutting edge.

· Do not wait until the tool tip smokes before starting coolant.

For machines without internal coolant, use wide external flood coverage from both sides of the cutter. The goal is not only to cool the insert but also to remove chips before they are re-cut.

Avoid Speed Loss

Speed loss is often invisible. The panel may show 4,000 RPM, but under load the real spindle speed may fall to around 3,700 RPM.

This small difference may not destroy roughing, but it can damage semi-finishing. At low feed per revolution, the chip becomes too thin, and the cutting edge starts pushing and rubbing instead of shearing.

For a 15 kW spindle, theoretical torque at 3,000 RPM is about 48 N·m. Higher torque values may be available only in lower-speed or peak-torque ranges, so the actual torque-speed curve should be checked from the machine specification.

· Normal cutting sound is usually a steady low-frequency hum.

· Insufficient speed or unstable cutting often creates a sharp, harsh sound.

· If the ammeter needle drifts or the spindle load fluctuates, reduce feed or depth by 20-30% before continuing.

To check whether speed is enough, calculate the minimum required speed first:

n_min = (Vc_target × 1,000) / (π × D)

Then compare this value with the machine's real loaded speed, not just the no-load panel speed. If the gap is more than 10%, adjust cutting parameters or change the tool diameter.

Choose the Tooling

Select Cutter Grade

Tool material selection is one of the biggest factors affecting surface finish and tool life in pre-hardened mold steel.

TiAlN-coated carbide is a common first choice for pre-hardened steel above 30 HRC. Its high coating hardness and high-temperature stability help resist crater wear and adhesion.

For P20 around 28-30 HRC, GC4240 or an equivalent steel-milling grade can be used as a practical reference. Cutting speed around 150-200 m/min is possible only when the setup is rigid and chatter is under control.

If the machine or fixture rigidity is marginal, choose a tougher fine-grain carbide grade and reduce cutting speed. Heat resistance alone is not enough if the edge keeps chipping.

The LJ-855 uses a BT40/CAT40-type interface depending on configuration. The tool holder, collet, and shank must match accurately.

Tool shank runout should stay under 0.02 mm for general machining. For finishing, 0.01 mm or less is a better target.

I have seen QC teams reject new tools when the runout exceeded 0.01 mm on the dial indicator. This is practical: above that level, eccentric load during high-speed cutting becomes easier to see on the workpiece surface.

Check Tool Runout

Radial runout is one of the most commonly ignored parameters when machining pre-hardened steel on the LJ-855.

Every 0.01 mm increase in runout can noticeably increase chip-thickness variation and cutting force fluctuation. In finishing, 0.02 mm runout can already create visible chatter marks.

Use a runout meter or dial indicator to measure the tool tip path while the spindle is slowly rotated by hand.

· Finish machining: runout ≤ 0.01 mm.

· Semi-finishing: runout ≤ 0.02 mm.

· Roughing: runout ≤ 0.03 mm.

With BT40/CAT40 holders, the contact condition between the tool holder taper and the spindle taper is a major source of runout.

A new or well-maintained machine may show runout around 0.005 mm. After repeated tool changes, taper wear, debris, or poor cleaning can raise runout to 0.015-0.02 mm.

If no precision instrument is available, a simple trial can still help. Machine a 45° chamfer and inspect the surface. If periodic waves appear and repeat with spindle rotation, check the spindle, holder, and insert seats.

Replace Worn Inserts

When coated carbide inserts wear, the coating usually fails first. Once the substrate is exposed, cutting force rises quickly and crater wear accelerates.

Replacement timing should not rely only on whether the edge "looks sharp." In pre-hardened steel, the edge can look acceptable while surface roughness and cutting power have already increased.

Using Sandvik GC4240 as a practical reference, roughing maximum VB can be treated as about 0.3 mm, while finishing should stay closer to 0.15 mm.^[4]

A common hidden failure occurs when the surface Ra increases by more than 0.3 μm while the insert edge still looks normal. In that case, the edge radius has usually grown, friction is higher, and the insert should be replaced.

· Inspect inserts after about 80 minutes of continuous machining.

· Inspect sooner if the material is above 32 HRC.

· Inspect the first part of each batch for critical cavity dimensions.

· If key dimensions drift by 0.01-0.02 mm, check insert wear immediately.

Plan Finish Passes

Leave Light Stock

The core strategy for finishing pre-hardened mold steel is light, stable cutting.

Leave 0.3-0.5 mm stock after roughing. This gives the finishing tool enough material to clean the surface without forcing it into a heavy cut.

If stock is more than 0.8 mm, finishing load becomes too high and vibration risk increases. If stock is less than 0.2 mm, the finishing pass may not remove the roughing stress layer or tool marks.

In 2023, I found an operator had reduced stock allowance to 0.15 mm to save time. During the finish pass, the tool bounced and the workpiece came out oversized.

For LJ-855 finishing, 0.3-0.5 mm stock is the safer working window for P20 pre-hardened steel.

If the previous roughing operation used different tools or a different clamping setup, add 0.1-0.2 mm stock to cover possible systematic error from tool setting, thermal movement, or fixture shift.

Limit Cut Depth

Depth-of-cut control in pre-hardened steel finishing is stricter than in aluminum or soft steel.

Recommended finish machining depth is 0.2-0.4 mm, with 0.5 mm treated as the practical upper limit for stable setups.^[7]

Radial engagement should usually stay below 30% of tool diameter.

· For a 10 mm tool, radial width should usually stay at or below 3 mm.

· For a 16 mm tool, radial width should usually stay at or below 4.8 mm.

· For a 20 mm tool, radial width should usually stay at or below 6 mm.

When depth exceeds 0.5 mm, radial force rises sharply. Tool deflection becomes more likely, and cavity dimensions may come out undersize or unstable.

Another risk is work hardening. Under low cutting speed and excessive depth, the surface can form a hardened layer around 0.05-0.15 mm thick.^[5]

To detect this problem, compare cutting load in the next pass with the baseline. If motor current rises more than 15-20%, reduce depth by 25-40% in the next pass.

Check Surface Finish

Surface roughness after machining is the most direct signal of whether the process is working.

For pre-hardened mold steel, the common target range is Ra 0.8-1.6 μm. With stable tooling, proper speed, and controlled runout, the LJ-855 can typically reach around Ra 1.0-1.2 μm.^[2]

If measured Ra exceeds 1.6 μm, check insert wear first, then spindle runout, tool holder contact, and fixture rigidity.

Surface quality affects more than appearance. Rougher mold surfaces require more polishing time and can carry a deeper residual stress layer after machining.

1. Inspect the surface visually with a 5× magnifier.

2. Measure Ra with a roughness meter and use the average of several points.

3. If the part is critical, check surface stress direction or residual stress with a suitable test method.

4. For mold faces requiring polishing below Ra 0.8 μm, reserve additional polishing allowance.

For every 0.4 μm increase in roughness above the Ra 0.8 μm baseline, polishing time can increase by about 15% in practical mold work.

Key Parameter Summary

In practical LJ-855 machining of P20 pre-hardened mold steel, stable results come from controlling all nine points together: hardness-based speed, cutting heat, real spindle speed, cutter grade, runout, insert wear, finish stock, cut depth, and final surface finish.