Drilling

Compiled 2026-04-04 · 40 chunks, 15 posts · drilling · speeds-feeds · chip-control · coolant · peck-drilling · deep-holes

Summary

Drilling is a fundamental machining operation that creates round holes by removing material with a rotating cutting tool. Success depends on proper speed and feed selection, effective chip evacuation, and understanding when to peck versus when to drill straight through. Modern carbide drills with through-spindle coolant have revolutionized the operation, often eliminating the need for pecking in many applications.

Speeds and Feeds

HSS Twist Drills

  • General starting point: 0.002-0.003" per revolution for drills under 1/8"
  • Small holes (.060" and under): 0.0001-0.0002" IPR, maximum 2000 RPM
  • Standard holes (.125"-.500"): 0.003-0.005" IPR
  • Large holes (over .500"): 0.005-0.008" IPR

Solid Carbide Drills

  • With through-spindle coolant: 0.005-0.008" IPR, no pecking required
  • Without coolant: Reduce feeds by 30-50%, add pecking
  • Surface speeds: 150-200 SFM for general purpose

Material-Specific Parameters

[[aluminum-6061]]: 250-400 SFM, 0.003-0.007" IPR

  • Shop floor reality: Machinists report calculators suggesting 25 IPM feeds that cause violent drilling - start conservative

[[304-stainless]]: 80-130 SFM, 0.002-0.004" IPR

  • Critical: Maintain constant feed to prevent [[work-hardening]]
  • With through-coolant carbide: 130 SFM, no pecking

[[4140-steel]]: 80-120 SFM, 0.003-0.005" IPR

  • H-13 (soft): 80-100 SFM for deep hole applications

Copper/Brass: Follow manufacturer SFM exactly, use carbide with coolant

  • Extremely grabby material - consistent parameters critical

Spot Drills

  • 142° carbide spot drills: 150-200 SFM, 0.003" IPR standard
  • Spotting depth: Only 0.030" deep - increase RPM for shallow cuts like chamfer mills
  • Never use 90° spot drills with 135° drill points - creates interference

Deep Hole Drilling

  • Gun drills: Start at 60 RPM, ramp to full speed in-cut
  • Long solid carbide: Titex 25XD style, 900-1000 PSI through-spindle coolant
  • Pilot sequence: Use stubby drill, then intermediate length, then full depth

Insert Drills

  • Kennametal indexable: Start at 25% feed until fully engaged
  • Large diameter (1-3/8"+): Expect violent entry/exit - normal behavior
  • Without through-spindle: Reduce manufacturer feeds by 30%

Pecking Strategy

When to Peck

  • HSS drills: Peck at 3× diameter initially, reduce to 1× diameter minimum
  • Deep holes: Any hole over 3× diameter depth
  • Poor chip evacuation: When flood coolant insufficient

Peck Depths

  • Minimum effective: 0.100" - smaller pecks create more heat
  • Small holes: 0.010" for holes under 0.125"
  • Rule: Start 3×D, reduce by 1×D each peck to minimum 1×D

When NOT to Peck

  • Through-spindle coolant carbide: Chips break naturally, coolant evacuates
  • Insert drills: Designed for continuous cutting
  • Short holes: Under 2× diameter typically

Chip Control and Coolant

Chip Evaluation

Look for "6's and 9's" - small broken chips indicate proper parameters. Long stringy chips mean:

  • Feed too low
  • Speed too high
  • Poor coolant flow

Coolant Requirements

  • Through-spindle pressure: 900-1000 PSI for deep holes
  • Flood coolant: Minimum for HSS, insufficient for deep carbide drilling
  • Concentration: Maintain proper mix for material type

Common Problems

Drill Breakage

Causes:

  • Excessive feed rate (0.007" IPR reported breaking drills instantly in aluminum)
  • Chip packing in deep holes
  • Wrong peck strategy
  • Work hardening in stainless

Solutions:

  • Verify actual feed per revolution, not just IPM
  • Check chip formation and evacuation
  • Use negative retract (only 0.10" above hole) to prevent re-entry damage

Hole Quality Issues

Wandering/oversized holes:

  • Use proper spot drill angle matching drill point
  • Check spindle runout
  • Reduce speed if drill flexing visible

Poor surface finish:

  • Usually appears after 1.5-2" depth in deep holes
  • Indicates drill deflection or coolant starvation
  • Consider drilling undersize and [[reaming]] to finish

Shop Floor Tips

Cycle Time Optimization

  • Skip spot drilling for self-centering carbide drills (135° point)
  • Rapid to depth: Program faster approach feeds to pre-drilled features
  • Batch operations: Use bolt circle macros for multiple holes

Programming Tricks

  • Retract feed: Use rapid, not drilling feed rate
  • Dwell time formula: 1.5 × 60 ÷ RPM for spot drilling operations
  • Load monitoring: Set limits 5-10% above normal load for consistent deep holes

Experience-Based Rules

  • "Most of the time I make up numbers, turn coolant on, and click green" - but start with handbook values
  • Every drill screaming indicates wrong parameters - not normal operation
  • 3XD rule: Universal starting point for peck depth calculation

Deep Hole Specific

  • Gun drill cycle: 60 RPM entry, full parameters in-cut, 60 RPM retract with coolant off
  • Pilot hole strategy: Clean up after pilot, test 0.500" depth for chip formation before full depth
  • Time expectations: 18 minutes for 1.75" × 0.060" hole in A2 is acceptable but optimize-able
  • [[reaming]] — finishing drilled holes for precision and surface finish
  • [[tapping]] — threading drilled holes
  • [[boring]] — enlarging and finishing drilled holes
  • [[chip-control]] — managing chip evacuation in deep holes
  • [[work-hardening]] — critical concern in stainless steel drilling
  • [[tool-wear-diagnosis]] — identifying drill wear patterns
  • [[surface-finish-problems]] — diagnosing poor hole quality