Introduction
Starting-point drilling calculator for RPM, feed per revolution, peck depth, and G81/G82/G83 cycle guidance across common twist, carbide, cobalt, and indexable drill workflows. Gun drilling and spotting/countersinking still need process-specific validation.
How It Works
Enter the planning inputs for this calculator, review the computed output, and compare the result against your machine limits, tooling, material, and shop-floor validation workflow.
Key Formulas
Use the formulas, assumptions, and process notes on this page to validate the result before applying it to a quote, investment case, or live machining setup.
How to Use
Follow the step-by-step guidance, worked examples, and caution notes on the page before locking in the final numbers for production or procurement.
Related Calculators
Use the related calculator links on this page when the current workflow needs a more specific model for speed, feed, cost, capacity, maintenance, or machine selection.
Drilling Feeds & Speeds Calculator 2026
Set starting-point drill RPM, feed per revolution, peck depth, and G81/G82/G83 cycle guidance for common hole-making workflows. Best for standard drill cycles, with clear guardrails for gun drilling, spotting, and countersinking.
Calculate Drilling Parameters
Drilling Feeds & Speeds: Complete Guide 2026
Drilling is its own process family. Feed is usually programmed in mm/rev or IPR, hole depth changes the safe speed window, and the correct canned cycle matters just as much as the RPM number. This page is built to give a disciplined starting point for twist drills, carbide drills, indexables, and deep-hole workflows before you prove out the exact machine, holder, and coolant setup on the floor.
What This Calculator Covers Best
- Common drilling jobs where tool type, hole diameter, depth, and material are already known.
- Feed-per-revolution planning, spindle RPM, peck-depth guidance, and a canned-cycle starting point for G81, G82, or G83.
- Cycle-time and tool-life estimation before moving into quoting with the machining time calculator.
- Not a replacement for machine-specific syntax, breakthrough control, holder runout checks, or OEM geometry recommendations for special drills.
Where This Page Needs Backup
- Gun drilling and very deep holes need dedicated machine alignment, guide support, and coolant-pressure validation beyond this calculator.
- Center drilling and countersinking use this page only as a speed/feed start point. Final angle, chamfer size, and spot depth still come from the print and tooling geometry.
- Precision holes should treat drilling as the roughing step, then move into boring or reaming logic before release.
Recommended Workflow
- Start from drill type, material, and actual depth-to-diameter ratio. If you only know cutting speed, convert it first with the RPM and cutting speed calculator.
- Use this calculator to set RPM, feed per rev, and whether the job needs G81, G82, or G83 style motion.
- Validate chip evacuation, coolant delivery, and hole tolerance. For H7-class or ream-ready holes, treat drilling as the roughing step and plan the finish process separately.
- When the hole-making process is stable, move to the formulas guide or machining time planning to price the full operation.
Understanding Drilling Parameters
Cutting Speed (Vc)
The surface speed at the outer diameter of the drill, measured in m/min or SFM.
Formula: Vc = (π × D × n) / 1000
Feed Rate (f)
How far the drill advances per revolution, measured in mm/rev or IPR.
Starting point: steel twist drills often begin near 0.015-0.025 × D, then adjust for depth, tolerance, and drill geometry
Spindle Speed (n)
Rotational speed of the drill, measured in RPM.
Formula: n = (Vc × 1000) / (π × D)
L/D Ratio
Hole depth divided by drill diameter. Critical for peck drilling decisions.
Guidelines: >3 = Peck drilling recommended
When to Use Peck Drilling
Peck drilling (G83 cycle) retracts the drill periodically to clear chips. Use it when:
- Deep holes: L/D ratio greater than 3:1
- Gummy materials: Stainless steel, aluminum, titanium
- Chip problems: Stringy chips wrapping around drill
- No through-coolant: HSS drills without coolant-through
- Blind holes: To ensure clean bottoms
Through-tool carbide drills can often push deeper before a full retract is needed, but that is still a machine-and-coolant decision. Treat the peck recommendation here as a safe process-planning default, not as a replacement for the drill maker's cycle sheet.
Peck Depth Guidelines
Drill Type Selection Guide
| Drill Type | Best For | Speed | Cost |
|---|---|---|---|
| HSS Twist | General purpose, low volume | 1× | $ |
| Cobalt HSS | Stainless steel, heat-resistant alloys | 1.3× | $$ |
| Solid Carbide | High-volume production, tight tolerance | 2.5× | $$$ |
| Coated Carbide | Maximum performance, difficult materials | 3× | $$$$ |
| Indexable | Large holes (>16mm), production | 3.5× | $$$$ |
| Gun Drill | Deep holes (L/D > 10) | 0.6× | $$$$$ |
Common Drilling Problems
Drill Walking / Wandering
Causes: No pilot hole, split-point not used, workpiece not perpendicular.
Solutions: Spot drill first, use 135° split-point geometry, reduce initial speed.
Drill Breakage
Causes: Chip packing, excessive feed, dull drill, misalignment.
Solutions: Use peck drilling, reduce feed, replace drill, check runout.
Oversized Holes
Causes: Spindle runout, drill wobble, excessive speed, dull margins.
Solutions: Check holder runout (<0.02mm), reduce speed, resharpen or replace.
Poor Surface Finish
Causes: Dull drill, improper coolant, excessive feed, chips re-cutting.
Solutions: Sharpen/replace drill, ensure coolant flow, reduce feed.
Programming Notes Before You Post Code
- G81: best for shallow through holes when chips clear naturally.
- G82: use for blind holes or bottom cleanup when a short dwell actually matters.
- G83: use when depth, chip packing, or stringy material makes full retract chip evacuation safer.
- Breakthrough behavior, retract planes, and dwell units vary by control. Verify syntax on the machine before running production.
Frequently Asked Questions
Use the steel answer on this page as a drilling start point rather than a universal hole-making rule. For mild steel with HSS drills, 20-30 m/min is a common range. Cobalt drills often start around 25-40 m/min, and coated carbide can run much higher when coolant and rigidity are there. Reduce speed as depth-to-diameter ratio climbs, and validate gun drilling, spotting, or countersinking separately because those processes are not governed by one simple twist-drill number.
Continue The Hole-Making Workflow
Use these next when drilling hands off to tapping, boring, spindle-speed conversion, or realistic cycle-time planning.
General Feeds & Speeds
Return to the main CNC feeds and speeds calculator for RPM, feed rate, chip load, SFM, MRR, and power context.
RPM & Cutting Speed
Convert SFM or m/min into spindle speed for the actual drill diameter.
Tapping Calculator
Use after drilling to validate thread-making speed, pitch feed, and tap drill workflow.
Boring Bar Calculator
Move here when drilling is only the roughing step and final hole size or finish depends on boring-bar rigidity.
Machining Time
Turn pecks, retracts, and hole count into realistic cycle-time estimates.