Series: Why Drill Bits Fail | Article 16
Keywords: incorrect drill RPM, drill bit speed, HSS drill bit RPM, drilling cutting speed, drill speed and feed, drill bit diameter and RPM, stainless steel drilling speed, feed per revolution, drill bit wear, drill bit breakage, stainless steel work hardening, why drill bits fail
A drill can fail early when its speed does not match its diameter, the workpiece and the feed. A useful RPM setting must be tied to all three. Simply turning the machine faster, or slower, does not guarantee a better hole.
This article focuses on HSS twist drills used in metal. HSS means high-speed steel. The reference values below explain the relationships; choose production settings from the data for the actual drill and material.
1 Understand speed before choosing RPM
| Term | What it means |
| Spindle speed n in RPM | How many revolutions the drill makes each minute. |
| Cutting speed Vc in m/min | The speed of the cutting edge at the drill outer diameter. |
| Diameter D in mm | Use the cutting diameter, not a reduced shank diameter. |
At the same RPM, a larger drill has a higher outer-edge cutting speed. At 1,000 RPM, a 10 mm drill runs at about 3.3 times the cutting speed of a 3 mm drill. These are calculated values, not recommended settings.
Figure 1 Same RPM, different cutting speeds. Calculated from Vc = πDn / 1000.
2 Excessive speed can shorten drill life
A drill may lose its edge before it breaks. Excessive speed and insufficient feed can shorten tool life. Excessive speed can also damage the outer corners. Coolant delivery and drill selection matter too.
A worn edge may need more force to keep cutting. Continuing the job without checking the edge and the process can turn a wear problem into a breakage problem. Record how the drill failed and where the damage started before deciding what to change.
3 Slower is not always better
Both excessive and insufficient drill speed can contribute to breakage. Small drills in stainless steel should not automatically be run at very low RPM.
There is also a feed issue. On a machine holding feed in mm/min, lowering RPM increases the distance advanced per revolution unless the feed setting changes as well. The worked example on the following shows why this matters.
A speed change cannot correct a loose workpiece, a damaged edge or a flute packed with chips. Those conditions need their own checks.
4 Stainless steel needs an effective cut
Austenitic stainless steels such as 304 and 316 can work-harden during drilling. Work hardening means strengthening caused by plastic deformation. It should not be described simply as heat making the steel harder.
Maintain suitable feed and avoid dwell or rubbing while the drill is in contact with the material. Chips must also be able to leave the hole. This calls for a sharp edge, suitable feed and effective chip removal. It does not mean applying unlimited force.
If a drill keeps rotating at the same spot without advancing or removing material, check the cutting conditions and edge condition. Repeated rubbing can make the next cut more difficult. Do not respond by increasing pressure without finding the cause.
What this means in practice
Treat RPM as one part of the drilling process. Review speed together with feed, coolant and chip removal. A correctly made drill still needs suitable operating conditions; an application problem also does not rule out a manufacturing defect.
5 An HSS reference for stainless steel
A general HSS cutting-speed reference range for stainless steel is 30 to 50 surface feet per minute, equivalent to 9.144 to 15.24 m/min. The table below converts that range to RPM. Use it to understand how diameter affects speed, then check the settings for the actual drill and material.
| Drill diameter |
At 9.144 m/min |
At 15.24 m/min |
| 3 mm |
970 RPM |
1,617 RPM |
| 6 mm |
485 RPM |
809 RPM |
| 10 mm |
291 RPM |
485 RPM |
| 13 mm |
224 RPM |
373 RPM |
Table 1 Calculated RPM, rounded to the nearest whole RPM. Conversion: 1 ft = 0.3048 m.
Figure 2 The same cutting-speed range requires lower RPM as diameter increases. The shaded band is a calculated reference range, not a tested safe operating zone.
This is a broad HSS reference range. It does not provide a dedicated setting for every stainless grade, hardness, coating or cobalt HSS drill. These values are not Jiacheng M35 or M42 product recommendations.
Use the actual drill manufacturer’s data first. Check material grade and condition, hole depth, coolant and machine capability. Do not copy a carbide speed chart to an HSS drill.
6 Match RPM with feed
Feed per revolution fn is the distance the drill advances in one turn, in mm/rev. Feed speed Vf is the distance advanced in one minute, in mm/min. Their relationship is:
Vf = fn x n
Suppose the machine holds feed speed at 60 mm/min. Changing only RPM produces the following values. This is an arithmetic example, not a drilling recommendation.
| Spindle speed |
Feed speed |
Feed per revolution |
| 1,200 RPM |
60 mm/min |
0.05 mm/rev |
| 600 RPM |
60 mm/min |
0.10 mm/rev |
| 300 RPM |
60 mm/min |
0.20 mm/rev |
Table 2 Calculated using fn = Vf / n. All three rows use the same feed speed.
Figure 3 With feed fixed at 60 mm/min, halving RPM doubles feed per revolution. Bar length shows axial advance per turn, not cutting force.
Reducing speed from 600 to 300 RPM doubles the advance per turn. If that new value is too high for the drill and setup, overload can still occur. Raising RPM while holding mm/min constant has the opposite effect and reduces advance per turn.
Check how the machine controls feed. With feed set in mm/rev, the controller normally changes mm/min with RPM to keep the selected advance per turn. Confirm the active mode and machine behavior before adjusting settings.
On a hand-fed drill, pressure is not a calibrated feed setting. The calculated values above cannot be converted directly into a recommended hand force.
7 Check the conditions before blaming RPM
One symptom can have several causes. Use the following checks to guide an investigation; the table does not diagnose a failed drill on its own.
| Observed problem | Checks to include |
| Short tool life | Speed, feed, drill selection and coolant reaching the point. |
| Damaged outer corners | Excessive speed, coolant and hard spots in the workpiece. |
| Sudden breakage | Chip packing, excessive feed, worn edge and secure clamping. |
| Oversized hole | Point centering, spindle condition and workpiece movement. |
For buyers and distributors, record the material grade and condition, drill model and diameter, hole depth, equipment, operating RPM, feed method and coolant. Add clear photos of the cutting edge, chips and failed section. This gives the supplier useful evidence for a fair comparison.
Suppliers remain responsible for material, heat treatment, geometry and batch consistency. Clear application guidance helps customers turn that product quality into repeatable drilling performance.
About this series
Why Drill Bits Fail is a technical series written by our production team. Each article focuses on one specific factor in drill bit performance — from raw material to packaging. The goal is simple: help buyers understand what they are actually buying, and which questions to ask.
Calculation notes
All chart points and RPM values are calculated, not measured performance results. Equations use D in mm, Vc in m/min, n in RPM, fn in mm/rev and Vf in mm/min.
Post time: Nov-03-2026