Drill Selection Guide

Compiled 2026-04-04 · 40 chunks, 15 posts · drilling · carbide · HSS · speeds-feeds · material-selection · coolant

Proper drill selection directly impacts hole quality, tool life, and cycle time. The choice between HSS, cobalt, and carbide drills depends on material, hole depth, machine capability, and production requirements. Modern carbide through-coolant drills have revolutionized [[drilling]] operations, but HSS still has its place for specific applications and older equipment.

Drill Types and Applications

HSS (High-Speed Steel) Drills

Best for: General purpose, older equipment, manual operations, materials under 30 HRC

  • Speed range: 50-150 SFM depending on material
  • Advantages: Forgiving, can be resharpened, handles interrupted cuts
  • Limitations: Lower speeds, frequent resharpening needed

Cobalt Drills (5-8% cobalt HSS)

Best for: Harder steels (30-45 HRC), [[304-stainless]], heat-resistant alloys

  • Speed range: 75-200 SFM
  • Feed rates: 0.002-0.008 IPR depending on diameter
  • Real machinist experience: "I would rather work with any other metal than copper. Follow the drill manufacturer recommendation for SFM and Feed rate in copper" but cobalt drills from Redline are "both good and cheap" for difficult materials.

Solid Carbide Drills

Best for: Production work, CNC equipment, consistent materials

  • Speed range: 200-800 SFM depending on material
  • Standard geometry: 135° split point, self-centering
  • Critical: Requires rigid setup and proper speeds - "I run an old Bridgeport that screams like a 2 year old at any speed over 3800rpm. So if I'm putting a small slot in aluminum I'll use HSS. I simply can't turn carbide fast enough"

Through-Coolant Carbide Drills

Best for: Deep holes, difficult materials, high-production

  • Advantages: No pecking required, superior chip evacuation
  • Coolant pressure: 900-1000 PSI minimum
  • Shop floor reality: "With through coolant carbide drills don't peck, just go straight through" and "if you're drilling at the correct speed and feed the chips will break on their own and the coolant will push them up and out the hole"

Speeds and Feeds by Material

Steel (Low-Medium Carbon)

  • HSS: 80-120 SFM, 0.003-0.006 IPR
  • Carbide: 250-400 SFM, 0.004-0.010 IPR
  • [[4140-steel]]: Reduce speeds 20% from low carbon values

Stainless Steel

  • 304 Stainless experience: One machinist conquered problematic 3/16" × 8.4" deep holes in [[304-stainless]] using:
  • 75 SFM
  • 0.0008 per tooth
  • 0.2" peck depth
  • 0.005" partial retract to break chips
  • Conservative approach: 130 SFM with through-coolant carbide, no pecking
  • Critical: Avoid [[work-hardening]] - maintain consistent feed, never let drill rub

Aluminum

  • HSS: 200-300 SFM, 0.005-0.015 IPR
  • Carbide: 500-1200 SFM, 0.008-0.020 IPR
  • [[aluminum-6061]]: Can handle aggressive parameters with good chip evacuation

Cast Iron

  • HSS: 100-150 SFM, 0.004-0.008 IPR
  • Carbide: 300-500 SFM, 0.006-0.012 IPR
  • [[cast-iron]]: Excellent machinability, moderate speeds work well

Hardened Steel

For hardened materials requiring carbide:

  • Surface speed: 100-200 SFM maximum
  • Feed: 0.002-0.005 IPR
  • Geometry: 135° split point essential
  • Real experience: 300 RPM or less for 3/4" hole through 2" of hardened steel

Spot Drilling Considerations

Modern reality: Self-centering carbide drills with 135° points don't require spot drilling for most applications. Forum consensus: "if I'm using self centering carbide drills with a 135deg nose I shouldn't have to spot drill first right?"

When to spot:

  • Angled or curved surfaces
  • Very precise hole location required
  • Drill larger than 1/2" diameter

Spot drill geometry: Use 142° spot drills, never 90°. "If you are spotting with a 90 or anything less than 140 you are damaging the drill"

Spot drill parameters:

  • Stainless: 150-200 SFM, 0.003 IPR for 1/2" diameter
  • Depth: 0.030" typical spotting depth
  • Many experienced machinists skip spotting entirely for carbide drills

Pecking Strategies

Traditional Pecking (HSS)

  • 3×D rule: First plunge 3× diameter, reduce by 1× diameter each cycle to minimum 1×D
  • Full retract: Clear chips completely
  • Example: 1/2" drill starts with 1.5" plunge, then 1.0", then 0.5" minimum

Chip Breaking (Carbide)

  • Partial retract: 0.005-0.010" to break chip
  • No full retract: Maintains cutting temperature
  • Through-coolant: Often eliminates pecking entirely

Deep Hole Drilling

For holes deeper than 5×D:

  • Gun drilling: Most reliable for extreme depths
  • Long carbide: 25×D possible with proper technique
  • Parameters example: H-13 steel, 185 SFM, 0.0015 IPR, 900-1000 PSI coolant

Insert Drills vs Solid

Insert Drills

  • Advantages: Replaceable tips, cost-effective for large sizes
  • Best for: Diameters over 15mm, production quantities
  • Geometry: Full-geometry inserts preferred over U-drills for deep holes

Solid Carbide

  • Advantages: Better concentricity, more geometries available
  • Best for: Smaller diameters, precision work
  • Regrinding: Possible but often not economical under 1/2"

Common Problems and Solutions

Drill Breakage

Causes: Wrong geometry for material, excessive speed, poor rigidity Solutions: Match drill type to application, verify setup rigidity, reduce speed before increasing feed

Poor Hole Quality

Causes: Dull drill, wrong speeds, inadequate coolant Solutions: Monitor [[tool-wear-diagnosis]], maintain proper parameters, ensure coolant flow

Work Hardening

Most common in: [[304-stainless]], [[inconel-718]] Prevention: Maintain consistent feed, never let drill rub, use sharp tools

Chip Evacuation

Problem indicators: Squealing, overheating, broken drills Solutions: Proper pecking, adequate coolant, correct geometry

Shop Floor Tips

  1. Speed vs Feed priority: "Sometimes you burn up drills constantly pecking instead of staying in cut" - maintain feed over reducing speed
  2. Coolant concentration: Critical for carbide - verify concentration and pressure regularly
  3. Setup rigidity: "The drill chuck on the turret is what would scare me" - ensure solid workholding and minimal overhang
  4. Economic reality: Quick napkin math shows carbide at 3× HSS speed can save $1000+ on deep hole jobs despite higher tool cost
  5. Machine limitations: Know your equipment - older machines may require HSS due to speed/rigidity limitations
  • [[drilling]] — fundamental drilling operations and techniques
  • [[tool-wear-diagnosis]] — identifying when drills need replacement
  • [[chip-control]] — managing chip formation and evacuation
  • [[work-hardening]] — preventing material hardening during drilling
  • [[surface-finish-problems]] — achieving required hole quality
  • [[toolholder-selection]] — proper drill holding methods