Calculate safe speeds and feeds for full-width slotting and keyway cutting. Slot milling engages the tool at 180° — feed rates must be reduced to prevent tool failure.
Full-width slotting (ae = D) is the most demanding milling operation. Feed rates must account for chip evacuation and heat concentration.
A programmer who treats slot milling like side milling will break tools. In side milling, the tool is engaged across 30-50% of its diameter — chips have room to form and exit, coolant reaches the cutting zone, and cutting forces are distributed across the engaged arc. In slot milling, the tool is buried in the cut at 180° engagement. Every flute is cutting from entry to exit. Chips must travel up both sides of the flutes simultaneously. Coolant struggles to reach the full cutting edge. Cutting forces are 2-3× higher than an equivalent side milling pass.
The fix is not complicated: reduce feed rate. But how much? Standard side milling feed rates must be reduced by 40-60% for slotting, depending on the material and slot depth. This calculator applies material-specific reduction factors so you don't have to guess.
In a full-width slot, the chip produced by each flute must travel the full length of the flute to exit the cut. In deep slots (depth > 2× diameter), the chip may travel 30-50 mm before clearing the tool. If the feed rate is too high, the chip volume exceeds the flute volume and the tool packs with chips. Packing causes the feed rate to stall, the spindle load to spike, and the tool to fracture at the flute root.
Two-flute tools evacuate chips better than four-flute tools in slotting because there is more physical space between cutting edges. For this reason, a 2-flute end mill at 60% of its normal feed rate may outperform a 4-flute end mill at 50% of its normal feed — the 2-flute tool clears chips more effectively and can sustain a higher effective feed.
For slots deeper than 1× tool diameter, pecking (multiple shallow passes) is recommended. Each peck should be 0.5-1× diameter deep, with a full retract between pecks to clear chips and allow coolant to reach the cutting zone. Single-pass slotting beyond 1.5× diameter depth requires reduced feed rates and should only be attempted with through-spindle coolant.
Pecking adds non-cutting time for retract and re-entry but allows higher feed rates during the cutting portion. The net cycle time often favors pecking for deep slots because the cutting feed can be 1.5-2× higher than single-pass feed. The Cycle Time Calculator can help determine the optimal number of pecks for your specific slot geometry.
Keyways are typically cut to tight tolerances (H7/h7 fits) and require a finish pass. The roughing pass should follow standard slot milling parameters with the finishing allowance of 0.2-0.5 mm per side. The finish pass takes 0.1-0.2 mm per side at 60-70% of the roughing feed rate to achieve the required surface finish and dimensional accuracy.
Keyway cutters (Woodruff cutters and keyseat cutters) have different geometry from standard end mills. They typically have fewer flutes (2-3) and a larger core diameter for rigidity. The feeds and speeds from this calculator are valid for standard end mills cutting keyways; for dedicated keyseat cutters, consult the manufacturer's recommendations.
Flood coolant at the tool entry point is the minimum requirement for slot milling in steel and stainless. The coolant stream must reach the cutting zone — not just the top surface of the workpiece. For slots deeper than 20 mm, through-spindle coolant at 20+ bar significantly improves chip evacuation and tool life. In aluminum, compressed air is often sufficient and preferred — coolant can cause thermal shock in aluminum at high feed rates.
MQL (minimum quantity lubrication) is effective for slotting in aluminum and mild steel. The oil mist reduces friction at the chip-tool interface without creating the thermal gradient that flood coolant produces. For stainless and titanium, high-pressure through-spindle coolant at 50+ bar is the only reliable coolant strategy for slotting.
What is slot milling? A milling operation where the tool is engaged across its full diameter (180° engagement), cutting a slot in a single pass. It is the most demanding milling operation due to restricted chip evacuation and high cutting forces.
How much should I reduce feed rate for slotting? Feed rate should be reduced by 40-60% compared to side milling at the same chip load. The exact reduction depends on material, slot depth, and tool geometry. This calculator computes the safe reduction automatically.
Can I use the same RPM for slotting as side milling? RPM should be slightly reduced (10-20%) for slotting to reduce heat generation at the tool center. The calculator's RPM value accounts for this reduction.
How deep can I cut in one pass for slot milling? For aluminum, up to 1.5× tool diameter in a single pass. For steel and stainless, limit single-pass depth to 1× tool diameter. For titanium, do not exceed 0.5× diameter per pass without through-spindle coolant.
What is the best flute count for slot milling? 2-3 flutes are preferred for slotting because they provide more chip evacuation space. 4-flute tools can be used for finishing passes where the depth per pass is low and chip volume is small.
When should I use trochoidal milling instead of slotting? For slots wider than 2× tool diameter, trochoidal milling with a smaller tool produces higher MRR and better tool life than conventional slotting with a full-width tool. Use the Trochoidal Milling Calculator to compare both approaches.
For slotting end mills with optimized flute geometry, check our High-Performance End Mills