Tool selection guide

Cylindrical Turning Face Turning and Inside Hole Turning: Tool Selection Guide

Three operations, three sets of cutting conditions. This guide is for engineers and buyers specifying turned parts who need to judge which insert, lead angle and holder will hold the drawing. Read it before you lock a process or a quote.

Get Instant Quote Talk to an Engineer

±0.005 mm toleranceRa 0.8–1.6 μm finish1 pc to 10,000+12-hour DFM reply

Cylindrical turning face turning and inside hole turning tool selection guide

On this page

1
Key takeaways
2
Tool geometry for cylindrical turning, face turning and bore work
3
What cylindrical turning face turning actually asks of the tool
4
Lead angle and approach angle: the biggest single lever
5
Inside hole turning: when the bar decides the tolerance
6
Insert grade and edge prep by material
7
What to verify before you award a turned-part order
8
Step by step: selecting the tool for a turned part

Quick verdict

Key takeaways

Lead angle decides the loadA 90° tool cuts a square shoulder but loads the tip. Use 45° for roughing long shafts.

Facing needs a different approach angleThe same holder that roughs Ø80 mm stock will chatter on a 3 mm flange face.

Bore tools are limited by length-to-diameterPast 4× diameter, deflection shows up as taper, not as a visible chip problem.

Inserts are chosen by material firstAluminium wants sharp edges and high rake; 17-4PH wants a tougher grade and lower speed.

Ask for the inspection reportTolerance on paper means nothing without a CMM report tied to the lot.

Selection matrix

Tool geometry for cylindrical turning, face turning and bore work

Pick the operation first, then the geometry. Values are common starting points, not fixed rules.

Operation	Typical lead / approach angle	Insert shape	Watch out for
Rough cylindrical turning	45°–75° lead	CNMG / SNMG	High radial force on slender shafts
Finish cylindrical turning	90°–95° lead	DNMG / VNMG	Tip chipping on interrupted skin
Face turning, open face	45° approach	CNMG	Unbalanced cut near the center
Face turning, thin flange	75°–90° approach	VNMG / DCGT	Chatter from low axial stiffness
Through bore, L/D < 3	0°–5° lead	CCMT / DCMT	Chip packing in blind corners
Deep bore, L/D 3–5	0° lead, positive rake	DCMT on carbide bar	Taper from bar deflection
Bore with interrupted cut	5°–15° lead	Tough grade CCMT	Edge chipping at cross holes
Fine finish on all three	Wiper geometry	WNMG wiper	Feed too high for the wiper to work

The verdict

Pick the geometry by operation, not by habit. Rough with 45°, finish with 90°, and treat every bore above 4:1 as a different problem. If the shop cannot explain why it chose the insert, the tolerance is a guess.

Get Instant Quote Talk to an Engineer

Basics

What cylindrical turning face turning actually asks of the tool

Cylindrical turning follows the Z axis along the part. The tool moves parallel to the axis of rotation, and the load is mostly radial. That radial load is what pushes a slender shaft away from the tool and turns a nominal Ø20 mm bar into a 20.04 mm beer barrel in the middle.

Face turning moves across the X axis. The tool travels perpendicular to the axis of rotation, and the load shifts toward the axial direction. The same insert that is stable on a shaft can chatter on a flange, because the part has far less stiffness in that direction.

Inside hole turning is a boring bar cantilevered out of the holder. The bar is the weakest element in the loop, not the insert. A Ø16 mm bar hanging 64 mm out of a holder is a 4:1 ratio, and that is already where deflection becomes measurable on the finished bore diameter.

So the three operations share a machine and a control, but they do not share tooling logic. Treating them as one setup is the most common reason a turned part passes the roughing stage and fails the final inspection.

1
Radial load dominatesCylindrical turning pushes the part away; support or reduce depth of cut.
2
Axial load dominatesFace turning pushes along the spindle; check the chuck and the part seating.
3
Bar stiffness dominatesBoring is limited by overhang, not by insert grade.

Lead angle

Lead angle and approach angle: the biggest single lever

Lead angle is the angle between the cutting edge and the feed direction. A 90° lead gives a square shoulder and puts the whole cutting force into the tip. A 45° lead spreads the same cut over a longer edge and thins the chip, so the heat leaves with the chip instead of staying in the insert.

For roughing a Ø60 mm 1045 shaft at 2.5 mm depth of cut and 0.25 mm/rev feed, a 45° CNMG runs cooler and lasts longer than a 90° tool. For a shoulder that must be square within 0.02 mm, the 90° tool is the only practical answer, and you accept the shorter edge life.

On face turning the approach angle does the same job in a different direction. A 45° approach on a large open face spreads the load; a 90° approach on a thin flange concentrates it and often produces a ringing cut.

One rule covers most work: rough with the smallest lead angle the feature allows, finish with the largest lead angle the surface allows.

1
45° leadRoughing, interrupted cuts, long shafts, lower radial force.
2
90° leadSquare shoulders, finishing passes, higher tip load.
3
Wiper insertFeed 0.15–0.25 mm/rev at light depth to reach Ra 0.8 μm.

Bore work

Inside hole turning: when the bar decides the tolerance

Boring bar deflection scales with the cube of the overhang. Doubling the overhang makes the bar eight times softer. That is why a Ø10 mm bar at 40 mm overhang behaves completely differently from the same bar at 80 mm, even with identical inserts and cutting data.

The practical limit for a steel boring bar is around 4:1 length-to-diameter for finishing work and 3:1 for roughing. Carbide bars and tuned anti-vibration bars push that further, but they cost more and still need a lighter depth of cut.

Deep bores also trap chips. A through bore with coolant through the bar clears chips well. A blind bore with a 0.5 mm corner radius at the bottom will pack chips unless you interrupt the feed or use a smaller nose radius.

If a bore is 60 mm deep and only Ø12 mm, we usually mill it or drill and ream it instead of boring it. Boring a hole that deep on a lathe is possible, but the cycle time and the scrap risk rarely make sense.

1
L/D below 3Standard steel bar, normal cutting data, no special setup.
2
L/D 3 to 5Carbide bar, reduced depth of cut, spring pass if needed.
3
L/D above 5Consider milling, EDM, or a two-sided setup instead.

Materials

Insert grade and edge prep by material

Aluminium 6061 and 7075 want sharp, uncoated or DLC-coated inserts with high rake. Cutting speed runs 300–600 m/min on a rigid setup. A honed edge that works well in steel will smear aluminium and build up edge on the flank.

Stainless 303 and 316 work harden in the cut. Keep the feed high enough to stay under the hardened layer, around 0.15–0.25 mm/rev, and never let the tool rub. 316 needs a tougher grade and a lower speed than 303.

Steel 1045 and 4140 run well with a CVD-coated insert at 180–250 m/min. 4140 at 28–32 HRC is the common pre-hard condition, and it will chip a fine-edge insert on the first interrupted pass.

Titanium Ti-6Al-4V and Inconel 718 are the cases where tool selection stops being about geometry. Both materials keep heat in the cut, so the insert needs a tough substrate, low speed and constant coolant. Ti-6Al-4V runs around 40–60 m/min; Inconel 718 runs 25–40 m/min with a round insert.

1
AluminiumSharp edge, high speed, keep the chip flying.
2
StainlessPositive rake, feed above the work-hardened layer.
3
TitaniumLow speed, high pressure coolant, no dwelling in the cut.
4
PlasticsPOM and PEEK cut clean with sharp polished inserts and air blast.

Buyer checks

What to verify before you award a turned-part order

Tool selection is only half the story. The other half is whether the shop can prove the result. Ask how the bore diameter is measured. A plug gauge tells you the bore is inside limits, but it does not tell you roundness or taper. A CMM report or an air gauge with a printout does.

Ask which machine the part will run on. A 4,000 mm turning center and a Ø400 mm rotary table handle different part families. A shop that quotes a long shaft without a steady rest is quoting a straightness problem.

Ask about the first article. A turned part with three operations and a bore usually needs a first-article inspection before the run continues, not after the parts are finished.

Ask what happens when the tolerance is not met. A shop that can rework, re-cut or replace without a change order is a different partner than one that argues about the drawing. GreatLight runs 100% inspection before shipment and supplies reports on request, which is the baseline you should expect from any supplier.

1
Measurement methodCMM or air gauge with data, not a plug gauge alone.
2
Machine assignmentMatch the part length and diameter to the machine travel.
3
First articleInspect before the run, not at the end.

Workflow

Step by step: selecting the tool for a turned part

Run these in order. Each step feeds the next.

1
1. Split the part into operationsList every cylindrical surface, every face and every bore with its tolerance. Mark which features are datum features. A bore that locates the part is not the same as a bore that only passes fluid.
2
2. Check the length-to-diameter ratio of each featureFor shafts above 6:1, plan a steady rest or a tailstock. For bores above 4:1, plan a carbide bar or a different process. This step decides the setup before any insert is chosen.
3
3. Match the lead angle to the featureSquare shoulder: 90°. Open roughing: 45°. Thin flange facing: 75°–90° with a light depth of cut. Deep bore: 0° lead with a positive rake.
4
4. Choose the insert grade for the materialAluminium: uncoated or DLC, sharp edge. Stainless: tough grade, positive rake, feed above 0.15 mm/rev. Pre-hard steel: CVD coated. Titanium and Inconel: tough substrate, low speed, high pressure coolant.
5
5. Set starting cutting dataRoughing: depth of cut 1.5–3.0 mm, feed 0.20–0.30 mm/rev. Finishing: depth 0.2–0.5 mm, feed 0.08–0.15 mm/rev. Wiper finish: depth 0.2–0.4 mm, feed 0.15–0.25 mm/rev. Adjust after the first two parts.
6
6. Prove the first articleMeasure the critical diameters, the shoulder squareness and the bore roundness. If the bore tapers, reduce the depth of cut and check the bar overhang before changing the insert.
7
7. Lock the setup and inspect at the endRecord the insert grade, the cutting data and the measurement method on the setup sheet. Keep 100% inspection on the critical features and sample the rest.

FAQs

Common questions on turning tool selection

Why does my turned diameter taper from one end to the other?

On cylindrical turning, a taper usually comes from part deflection, not from the insert. A slender shaft pushes away from the tool, so the middle of the part cuts oversize while the supported ends stay on size.

Check the length-to-diameter ratio first. Above 6:1, use a steady rest or a tailstock. If the taper is small and consistent, a spring pass at the same setting often brings the diameter back into tolerance.

Can one insert handle cylindrical turning, face turning and boring?

One insert body can sometimes cover two of the three, but not all three in a production setup. The lead angle and approach angle that work on a shaft are wrong for a thin flange face.

For short-run prototype work, a CNMG or DNMG insert with a general-purpose grade can rough and finish a simple part. For a run of 500 pieces, separate the operations and choose geometry per operation.

How do I stop chatter when facing a thin flange?

Reduce the axial load. Use a 75°–90° approach angle, lower the depth of cut to 0.3–0.5 mm and keep the feed up so the tool does not rub. Support the part with a tailstock or a chuck jaw close to the face.

If the flange rings at any depth of cut, the part is the problem, not the tool. Add a support or turn the flange before the part is thin.

What surface finish can turning reach without grinding?

On a rigid setup with a wiper insert, turning reaches Ra 0.8–1.6 μm as a normal production finish. Fine turning with a sharp insert and a light feed can reach Ra 0.2–0.8 μm on aluminium and free-machining steel.

Below Ra 0.2 μm, grinding or lapping is usually the practical route. For most bearing seats and seal surfaces, Ra 0.8–1.6 μm is enough.

Does the shop need a 5-axis machine to turn a complex part?

Not for the turning itself. Turning is a 2-axis operation. A 5-axis machine helps when the part has features that cannot be reached from one setup, such as angled holes or cross features.

For a turned part with a few milled flats or cross holes, a mill-turn center or a 4-axis setup covers most cases at a lower cost than a full 5-axis cycle.

What information should I send with an RFQ for a turned part?

Send the 2D drawing with tolerances and surface finish, the 3D model, the material and the quantity. Note which features are critical and which are cosmetic.

If you have a preferred inspection method or a required report, say so in the RFQ. It changes the quote and it avoids a discussion at the end of the run.