Changing rpm or feed after a drill begins to wear, chip, or make poor holes can feel like the fastest corrective action. It can also create a misleading result. A change that reduces breakage may increase burrs, worsen size control, slow the cycle, or shift the load to another part of the tool. In production, a useful cutting condition is one that produces accepted holes consistently, not merely one that lets a drill survive the next few cycles.

This guide explains how to establish carbide drill speeds and feeds for CNC drilling. It covers cutting speed, feed per revolution, chip thickness, coolant delivery, hole depth, entry and exit condition, machine rigidity, and a controlled validation sequence. It is a method for applying tool-supplier starting data to a real process, not a universal parameter chart.

Direct answer: Use cutting speed to manage the thermal and wear environment, and feed per revolution to manage chip thickness, thrust, and mechanical loading. Start with the specific tool supplier's recommendation for the actual drill and material group, then adjust only after checking toolholding, coolant, chips, hole geometry, and stability. Change one controlled variable at a time and confirm both tool condition and accepted-hole quality.

If the current process is unstable, Discuss Your Application with XRZ before changing several settings at once. Provide the drill specification, material grade and condition, hole drawing, speed, rpm, feed per revolution, cycle, coolant, holder, runout record, tool-life history, chips, and photographs of the tool and holes.

Separate Cutting Speed from Feed per Revolution

Cutting speed is the speed at the cutting edge relative to the workpiece. In a rotating drilling operation, rpm is calculated from cutting speed and drill diameter. Feed per revolution is the axial advance of the drill in each revolution. Feed rate per minute is then derived from feed per revolution and rpm.

The basic relationships are:

  • rpm = cutting speed divided by the drill circumference using a consistent unit system;
  • feed rate = rpm x feed per revolution.

The formulas are simple. The application is not. The same rpm can represent very different cutting speeds at different diameters, and the same feed per revolution can create very different edge loading when drill geometry, material condition, entry, and rigidity change. For this reason, record speed and feed in units that can be traced back to the cutting condition rather than retaining only a machine-program line.

Do not treat speed and feed as a single “aggressiveness” setting. Cutting speed primarily affects temperature, friction, and wear behavior. Feed per revolution changes chip thickness, thrust, torque, and the tendency to rub or overload the edges. When both are changed together, the production result is difficult to interpret.

Core Formulas (Keep Conventions Straight)

n = (1000 × Vc) ÷ (π × D) — spindle speed (rpm) from cutting speed Vc (m/min) and diameter D (mm).

Vf = n × fn — table feed (mm/min) from feed per revolution fn (mm/rev).

Confirm mm/rev vs mm/tooth before entering data. These identities do not create a universal starting table—they only convert units once a starting reference is chosen for the material family and depth class.

Begin with a Traceable Starting Point

Use the data supplied for the exact drill family, diameter, material group, coating, coolant arrangement, and depth range as the first input. Sandvik Coromant notes that recommended speed and feed for deep and micro drilling are reference values and may need adjustment for the specific application. That is the right expectation for any production setup: a recommendation is a controlled starting point, not proof that the process is ready.

Before running a test, record:

  • tool maker, drill designation, diameter, flute length, coating, and coolant configuration;
  • workpiece material, grade, condition, hardness where relevant, and entry surface;
  • hole diameter, depth, type, tolerance, exit condition, cross holes, and any chip trap;
  • rpm, cutting speed, feed per revolution, feed rate, cycle, dwell, retract, and entry/exit commands;
  • spindle, holder, projection, measured runout, workholding, and machine alarms or load information;
  • coolant type, concentration, delivery method, pressure, flow, and filtration;
  • tool condition, chip appearance, hole-quality result, and accepted-hole count.

The initial setup should also be physically credible. Sandvik Coromant's drilling guidance places hole requirements, component stability, machine capability, coolant, workholding, and toolholding ahead of a simple speed-and-feed choice. A parameter change cannot correct a loose fixture, contaminated collet, blocked coolant path, unsuitable drill type, or unsupported breakthrough. Use the existing carbide drill selection guide when the unresolved question is tool construction or material suitability rather than cutting data.

Material Families as Starting References

Group the job by material family before copying any catalog number. Treat supplier windows as starting references only—not universal tables or life guarantees.

Product hub for custom geometry: solid carbide drill.

Use Speed to Control the Thermal and Wear Environment

Increasing cutting speed can change heat generation, friction, material adhesion, and wear rate. The correct response to a wear problem is therefore not always “reduce speed,” and a higher speed is not automatically more productive. Material behavior, coating, coolant access, edge condition, and the measured wear pattern determine which direction deserves testing.

CERATIZIT's solid-carbide-drilling guidance provides useful mechanism-based examples. It identifies excessive cutting speed as one possible contributor to significant flank wear, while built-up edge can be associated with cutting speed that is too low, excessive honing, or an uncoated edge. These are diagnostic relationships, not fixed settings to copy across materials. The same visible symptom must be checked against chip form, cooling, geometry, and stability.

For a speed review, ask:

  • Is the drill showing progressive flank wear, adhesion, discoloration, plastic deformation, or a different mechanism?
  • Does coolant actually reach the point at the required depth?
  • Is the material condition consistent from one batch or casting location to another?
  • Did the issue start after a change in coating, coolant concentration, cycle, tool projection, or workholding?
  • Is the tool operating through a casting skin, work-hardened layer, or interrupted feature that changes local heat generation?

Make the smallest justified test change, and keep feed, geometry, coolant, and cycle constant during that test. Inspect the drill before catastrophic failure rather than deciding from the last broken tool alone.

Use Feed to Produce a Stable Chip, Not to Chase a Number

Feed per revolution must be sufficient for the cutting edges to form a chip rather than spend an extended period rubbing. At the same time, excessive feed can increase thrust, torque, corner load, and the likelihood of chipping or deflection. The useful feed is the one that produces stable chips and hole quality under the actual rigidity of the setup.

Low feed can be a hidden source of heat and accelerated wear. CERATIZIT includes insufficient feed among possible contributors to major flank wear. High feed can create a different failure mechanism: overload at the point, corners, or chisel edge; unstable entry; or a large torque increase as chips cannot leave the hole. This is why a single recommended feed cannot be separated from depth, chips, coolant, and entry condition.

Watch the evidence while testing:

  • chips that become long, tangled, crushed, or packed in the hole;
  • one flute carrying visibly different chips from the other;
  • rising spindle load at a repeatable depth;
  • corner chipping at first engagement or at breakthrough;
  • a polished or heat-affected edge that suggests rubbing;
  • burr growth, hole-size change, wall scoring, or a deteriorating downstream operation.

Do not reduce feed automatically when corners chip. CERATIZIT associates broken corners with unstable conditions, significant runout, and interrupted cutting as well as feed. First confirm whether a mechanical or entry problem is concentrating load on one edge. The solid carbide drill failure guide provides the inspection sequence when the evidence points to breakage rather than initial parameter setup.

Depth Ratio (L/D) Notes

Express depth as a multiple of diameter (×D / L/D). The same starting Vc and feed behave differently at ≈3×D, 5×D and 8×D because chip volume, heat and side load rise together. Deeper holes usually need more flute volume, controlled peck and often through-coolant—not only a lower speed. Guide: deep-hole L/D, peck & chip escape.

Coolant and the Drilling Cycle Change the Real Cutting Condition

The program may show one speed and one feed, but the cutting condition changes if chips are trapped, coolant does not reach the point, a peck cycle repeatedly recuts chips, or the drill spends time dwelling and rubbing. Blind holes, deep holes, cross holes, interrupted exits, and long-reach tooling all need to be considered before accepting a parameter recommendation.

For internal-coolant drills, verify that the machine can provide the required delivery conditions and that the passages, filtration, and coolant condition support the process. For external coolant, observe whether it reaches the cutting zone and whether it helps clear the actual chips. Coolant should be reviewed as part of the geometry-and-cycle system, not as an isolated checkbox.

Hole entry and exit deserve separate records. An angled or irregular surface, casting skin, incomplete support, cross-hole intersection, and thin-wall breakthrough can create loads that are absent in a stable test coupon. A feed that works at full engagement can require a controlled approach at entry or exit. The change must be validated at the exact feature where the failure begins.

Through-Coolant Pressure and Flow

When flood cannot reach the cutting zone, internal coolant pressure and flow decide whether chips leave before packing. Record bar/psi, filtration and holder sealing. Product path: through-coolant carbide drills. Knowledge: when flood is not enough.

Build a Controlled Speed-and-Feed Validation Plan

The goal is not to find a plausible number. It is to show that a controlled change improves the complete process without shifting a quality or cost problem downstream.

  1. Freeze the baseline. Record the current tool, material, machine, holder, coolant, program, chips, tool condition, and accepted-hole result.
  2. Classify the dominant issue. Separate thermal wear, adhesion, rubbing, mechanical overload, chip packing, unstable entry, and toolholding error as far as evidence allows.
  3. Check the system before the parameters. Inspect runout, holder condition, projection, fixture support, coolant path, and hole features.
  4. Choose one variable. Change cutting speed, feed per revolution, entry feed, cycle, or another controlled item, but not several at once.
  5. Run a defined test quantity. Select a quantity sufficient to inspect an early trend; the correct number depends on the application and is not a universal XRZ requirement.
  6. Inspect tool and holes at intervals. Record edge condition, chips, load, diameter, position, surface, burrs, and downstream result.
  7. Compare cost per accepted hole. Include tool use, machine time, tool changes, inspection, scrap, and rework.
  8. Set a production control. Define the change point, inspection interval, coolant check, and action triggered by abnormal wear or chip behavior.

XRZ's sample validation process can be used when a tool geometry or process change needs a recorded comparison. The final decision should be based on the whole route, including quality and production burden, rather than purchase price or a short test alone.

Rigidity, Stickout and Runout

Assembled runout and excessive stickout can invalidate any starting speed/feed. Measure TIR at an agreed gauge length, shorten projection where possible, and fix the holder before chasing rpm. Specialist page: stickout, runout & toolholders.

Parameter Boundaries: When the Tool or Process Must Change

If speed and feed tests do not produce stable chips and accepted holes, do not continue narrowing the range indefinitely. The underlying limitation may be the tool geometry, flute length, coolant arrangement, hole form, machine rigidity, fixture, or the choice of drilling process.

A difficult hole may require a custom solid carbide drill designed for its material, depth, step, and coolant environment. A large diameter or power-limited machine may favor another drilling strategy. A hole with a critical finished-bore requirement may be better treated as a drilling-plus-finishing route, with a suitable reamer, boring process, or honing operation. The correct answer is the process that produces the functional hole reliably.

Common Speeds-and-Feeds Mistakes

  • Copying a universal chart without material family, depth ×D or coolant reality
  • Raising speed to “fix” short life without classifying wear vs packing vs runout
  • Feed too low → rubbing, heat, BUE or work-hardening at entry
  • Changing speed and feed together so the result cannot be attributed
  • Ignoring exit/entry features that only exist on the production part
  • Skipping breakage diagnosis: why solid carbide drills break

Information to Send XRZ for a Cutting-Data Review

Send the part drawing, material designation, drill specification, tool photographs, chip photographs, measured hole result, current cutting data, program details, machine and holder information, runout measurement, coolant details, current accepted-hole count, cycle time, scrap, and production volume. Send Your Drawing and the baseline evidence to request a preliminary review. Any recommendation should be confirmed through application-specific sample validation before production release.

Frequently Asked Questions

Should I increase speed when carbide drill life is short?

Not automatically. First identify the wear mechanism, coolant condition, material behavior, geometry, and stability. Excessive speed can contribute to flank wear, while low speed can contribute to built-up edge in some applications. Test one change against recorded evidence.

Can feed that is too low damage a carbide drill?

Yes. Too little feed can promote rubbing, heat, and flank wear. The correction depends on material, drill geometry, depth, coolant, rigidity, and the observed wear pattern.

Why do parameters work in a test but fail in production?

Production may have a different holder, runout, projection, fixture, material condition, coolant delivery, entry condition, or chip-removal path. Compare the complete system, not only rpm and feed.

Should speed and feed be changed together?

Not in a diagnostic validation test. Keep other controlled variables stable so the result can be attributed to the single change. A later optimization may use a broader design of experiment, but the baseline must remain traceable.

Is there a universal carbide drill speed chart?

No. Charts are starting references by material family. Depth, coolant, rigidity and the actual drill geometry change the window. XRZ does not publish fake life % or Nx guarantees.

Where should I send a drill RFQ after parameters fail?

Use the solid carbide drill RFQ checklist and Engineering RFQ. Include material, ×D, coolant, runout and failure photos. Product paths: solid carbide drill, aluminum, stainless, through-coolant.

CARBIDE DRILL SPEEDS & FEEDS

Set Parameters — Then Spec the Drill

Use process evidence for speed and feed, then route to a custom solid carbide drill when geometry, coolant or depth exceeds catalog limits.

Solid Carbide Drill · RFQ checklist · Engineering RFQ · why drills break

Technical References

Engineering review: Jiack Liu, Engineering Director. Review completed.