What does this page cover?

AgileMakeAI provides online manufacturing services for CNC machining, 3D printing, sheet metal, rapid prototyping, injection molding, AI quoting, file upload, order collaboration, and delivery tracking.

Which manufacturing keywords does this page cover?

This page covers online manufacturing, on-demand manufacturing, instant quote, precision machining, CNC machining, 5-axis machining, CNC milling, 3D printing.

What does this page cover?

AgileMakeAI provides online manufacturing services for CNC machining, 3D printing, sheet metal, rapid prototyping, injection molding, AI quoting, file upload, order collaboration, and delivery tracking.

Which manufacturing keywords does this page cover?

This page covers online manufacturing, on-demand manufacturing, instant quote, precision machining, CNC machining, 5-axis machining, CNC milling, 3D printing.

CNC Turning Process and DFM: How to Set Workholding, Relief Grooves, and Tolerances

What CNC turning is actually solving: one-shot forming of revolved bodies

Take the most common revolved-body drawing: a φ20h7 journal at one end, a M16×1.5 external thread in the middle, a φ8 bore at the tail with an R1 fillet at the bottom, and an overall length of 120 mm. Almost every contour line on this drawing is distributed around the same axis. CNC turning handles this type of part: the workpiece is clamped in the spindle chuck and rotates at high speed, while the tool only performs single-point feed; the outer diameter, face, grooving, thread, and bore are formed one by one in a few passes.

Its value isn't in the word "precision," but in the fact that revolved surfaces can be formed in one shot. To mill the same section of outer diameter, the tool needs to follow an interpolated path around the workpiece, and the surface is the result of overlapping tool marks; turning, by contrast, is generated by the workpiece itself rotating, so cylindricity and coaxiality are inherently determined by spindle accuracy. A judgment repeatedly mentioned in the source material is: if the feature lies on a revolved surface, go with turning; only if it lies on a flat face, a side hole, or an asymmetric cavity does milling or turn-mill come into play.

When it comes to the actual choice, you can first do three self-checks:

Look at the feature faces: outer diameters, faces, bores, conical surfaces, threads, annular grooves—these are turning's home turf. Flat faces, keyways, side counterbores, and irregular cavities belong to milling.
Look at whether a second setup is needed: if the part is "a flat on a shaft + an eccentric hole at the shaft end," turning it and then moving to a milling machine for another clamping can drop coaxiality from 0.02 to over 0.05. That's where the value of turn-mill's reduced setups comes in.
Look at batch size and shape: for a single piece, an odd shape, or internal flow channels—3D printing or silicone casting may be faster; only when true revolved-surface precision is needed and the quantity is a few to a few dozen does CNC turning hold up.

A common misjudgment in the industry is equating "has a shaft" with "must be turned." For a short shaft with a flange, the bolt holes, locating spigot, and side flats on the flange often consume more machining time than the journal itself. If these features make up more than half of the drawing, don't rush to quote it as turning—having a process engineer classify by feature and then decide the operation combination will save rework and arguments later.

How to choose between turning and turn-mill: first see which face the feature lies on

It's not uncommon for the same revolved-body drawing to be quoted at double the price. The reason is often not the material or tolerance, but "which face these features lie on." To judge turning, milling, or turn-mill, you don't need to memorize machine models first—first classify the features on the drawing by position.

Revolved surfaces, faces, external threads, bores—these features around the spindle axis are CNC turning's natural territory. The workpiece rotates and the tool feeds in a straight line; one pass completes a section of revolved surface with no tool marks from overlapping passes, and roundness is easy to keep stable. As long as the main body of the part is a revolved body, turning is usually the first and lowest-cost operation.

The trouble lies in another class of features: side flats, eccentric holes on a flange, cross holes perpendicular to the axis, and keyways on the outside. They aren't on revolved surfaces, and a lathe with a single-point tool can't produce them. The traditional approach is to flip the part for a second setup on a milling machine, or make an eccentric fixture so the lathe can "barely" machine it. A second setup means re-alignment, and both coaxiality and position tolerance gain another layer of error transfer. A common industry practice is: as long as there are more than two or three side features, or there are position-tolerance requirements relative to the spindle, go straight to milling or turn-mill rather than forcing it on a lathe.

A criteria table: feature position determines operation assignment

Once you map features to operations, the trade-offs become clear:

Outer diameters, faces, conical surfaces, bores, external/internal threads—CNC turning can complete them in one setup, with no extra operation needed.
Side flats, keyways, flange eccentric holes—assign to milling, or complete them in one setup using the C-axis/powered tool turret of a turn-mill.
Cross holes perpendicular to the axis, small radial holes—turn-mill can eliminate the second setup; if there are few and their positions are loose, you can also turn first and drill later.
Non-revolved contours (irregular outer profiles, thin sheets)—go directly to milling, 3D printing, or sheet metal; don't force turning.

The value of turn-mill in one sentence: compressing features that would otherwise require two or three setups into a single setup. Fewer setups mean less accumulated error, and coaxiality and position tolerance are easier to achieve. It's not about showing off the number of axes or a rotary table. If all the key features on the drawing are on revolved surfaces, using a five-axis turn-mill actually makes a simple part expensive. Conversely, if there are many side features and tight position tolerances, the alignment time and scrap rate saved by fewer setups are often worth more than the machine's hourly rate.

Common CNC turning operations: which features on the drawing the 10 types of actions correspond to

When reading a drawing, if you can map line types directly to tool motions, drawing review becomes much faster. CNC turning is nothing more than ten basic actions, each corresponding to a specific feature on the drawing.

Outer diameter turning: follow the longest outer contour line, from the face to the shoulder. Use an external turning tool; radial depth of cut and feed determine surface roughness, and tool deflection is most pronounced when the length-to-diameter ratio is large.
Face turning: follow the plane perpendicular to the axis. The face is the datum for all subsequent length dimensions; if the face isn't flat, everything after it is off.
Grooving: a section on the drawing that suddenly narrows in width, usually a relief groove, retaining ring groove, or O-ring groove. Grooving tools have poor rigidity, and when the groove width-to-depth ratio exceeds 3:1, chatter is likely.
Parting off: the line at the end of the bar stock perpendicular to the axis, separating the part from the stock. The parting tool is the thinnest, so the feed must be slow.
Thread turning: lines marked M, Tr, G, or with a thread profile angle. The threading tool must make multiple passes; pitch and thread depth determine the number of passes, and fine threads are more prone to cross-threading than coarse threads.
Boring: the bore dimension line. The longer the boring bar overhang, the worse the rigidity; when the depth-to-diameter ratio exceeds 4:1, the bore mouth tends to be large and the bore bottom tends to be small.
Reaming: when a bore is marked with H7 or H8 precision, a reamer is often needed after turning to finish it; this is a semi-finishing method.
Knurling: The drawing shows a diamond or straight knurl symbol, used for grip on handles. After knurling, the outer diameter will grow, so allowance must be reserved.
Form turning: For arcs, conical surfaces, and spherical contours, use a form tool or CNC interpolation to cut in one pass. The tool nose radius must match the contour.
Drilling: For axial holes such as center holes and oil holes, this can be done on a lathe with a tailstock or turret drill. Eccentric holes require dedicated fixtures.

Among these ten types of operations, the ones most sensitive to tool rigidity are grooving, parting off, internal boring, and thread turning. Their common trait is a slender tool shank or concentrated force at the tool tip, so spindle speed, feed, and depth of cut must all be tightened together. External and face turning are relatively forgiving, but once the length-to-diameter ratio goes up, tool deflection still appears. When reviewing a drawing, first count how many types of operations appear on it, then assess whether the workholding and toolpath conflict.

Workholding and datums: the most underestimated aspect of CNC turning

Coaxiality and face perpendicularity on the drawing are ultimately realized by the jaws and datum surfaces. In the same CNC turning process, completing the part in one setup versus flipping it for two setups can result in a coaxiality difference of an order of magnitude. To judge whether a rotational part drawing is easy to make, first ask: where is the datum, and how many setups are needed?

Applicable boundaries of common workholding methods

The three-jaw chuck is versatile and provides strong clamping force, but repeat positioning is poor, with runout often in the 0.02–0.05 mm range. It suits rough turning and general-precision outer diameters. Soft jaws are bored to the workpiece profile, improving positioning accuracy by a step, and are often used for finish turning and maintaining consistency in secondary setups. Spring collets clamp evenly with low runout and are an efficient choice for slender shafts and small-diameter parts, but the clamping range is narrow—one collet corresponds to one diameter range.

For internal bore locating, use a mandrel (arbor): first turn the datum bore, then mount it on the mandrel to turn the outer diameter, transferring the bore datum to the outer diameter. This is a conventional practice for high coaxiality requirements. Face driving (face driver dogs) suits turning the full length of a shaft in one setup, eliminating the need to flip. Workpieces with large length-to-diameter ratios must use a steady rest or follow rest: the steady rest supports the static section, while the follow rest moves with the tool to support the cutting point. This is key to controlling deflection and taper.

Flipping to turn the other end: how datum transfer accumulates errors

Typical scenario: one end of a stepped shaft is clamped and turned, then released and flipped to clamp the other end to turn the remaining outer diameter. The radial locating datums differ between the two setups, and chuck runout, clamping deformation, and face contact errors all stack onto coaxiality. If the datum surface from the first setup is itself not flat, the axis in the second setup will be off. The result often shows as out-of-tolerance coaxiality between the two ends and noticeable runout at the middle step.

The countermeasures are practical: critical rotational surfaces that can be completed in one setup should be done in one setup as much as possible. When flipping is unavoidable, in the first setup also turn a reusable locating datum (such as a finish-turned outer diameter or bore), and in the second setup locate on that datum using a mandrel or soft jaws. Leave finishing allowance on critical mating surfaces and finish-turn them uniformly after flipping. Writing the "datum" into the drawing or process card saves more trouble than fitting after the fact.

Length-to-diameter ratio: a common criterion for workholding plans

Common industry experience: with an overhang length-to-diameter ratio (overhang length / diameter) within 3 times, a standard chuck can usually hold it without much issue; at 4–6 times, the risk of deflection and taper rises noticeably, and a steady rest or follow rest is usually needed; beyond 6–8 times, most cases require a follow rest combined with small depth of cut and low feed, or a different process route. These are only order-of-magnitude references for judgment. Specifics must be confirmed against drawing tolerances, material rigidity, and the actual machine and tooling—they cannot be treated as guaranteed values.

For thin-walled parts, the opposite also applies: clamping force itself deforms the workpiece, which springs back after release. In this case, axial clamping, increased contact area, and light clamping in multiple stages are often more effective than simply increasing clamping force. Once the workholding plan is set, whether CNC turning can reproduce stably is largely determined.

Schematic of datum transfer in CNC turning when a three-jaw chuck grips a stepped shaft and a second setup after flipping, with the direction of accumulated coaxiality deviation marked

Undercuts, thread runout, and bore bottoms: not reproducible if not specified on the drawing

Turning tools are physical bodies with geometry, not mathematical points. The tool nose radius, lead angle, and end cutting edge angle determine where it can cut and where it cannot. If the drawing only shows an outer diameter and a thread line, the machinist will decide on their own how wide the undercut should be, where the thread stops, and how large the fillet at the bore bottom should be. The same drawing sent to a different shop may produce parts that none of which fit together. The following features are typical "must specify" types—not specifying them does not mean they cannot be made, but that making them is not reproducible.

External undercut: width and depth determine whether the tool can "get through"

When a large-diameter section of a stepped shaft transitions to a small-diameter section, if the step is a right angle, the minor cutting edge will rub against the end face of the large-diameter section when the tool reaches the root of the step. Therefore, an undercut must be cut at the root. There are two numbers that must be specified: groove width and groove bottom diameter. The groove width must be greater than the width of the grooving tool head, otherwise the tool cannot enter; the groove bottom diameter must be smaller than the position that the mating part's chamfer or bore end face is allowed to pass. Common industry practice is to take the groove width as 1.5–3 times the tool width and the depth slightly greater than the thread minor diameter or the mating part's fillet radius. Specifics depend on the actual tool head in the tool library and the mating part dimensions.

Thread runout: cannot be screwed all the way in if not specified

When an external thread is turned to the root, the tool cannot disappear instantly; there must be a transition zone where it gradually cuts in, cuts out, and the thread depth is insufficient—this is thread runout. If the drawing does not show an undercut at the thread root or specify the allowable runout length, the machinist can only handle it according to the natural runout of a standard threading tool, which may be 2–3 times the pitch. If the mating part has an internal thread all the way to the bottom with no clearance space, it will bottom out hard. The way to judge: first look at the distance from the mating part's internal thread end face to the root, then decide whether to add an undercut or specify the allowable runout length on the drawing.

Bore bottom: fillet radius and overtravel space

When boring to the bottom of a hole, the boring tool also has a tool nose radius. If the drawing shows a right-angle bore bottom, the actual part will inevitably have a fillet, with a radius roughly equal to the tool nose radius. If the mating shaft end has a chamfer or fillet, this bore bottom fillet must be less than or equal to the shaft's clearance dimension; otherwise the shaft cannot be installed all the way to the bottom—the dimensions look correct, but assembly is short by a bit. It is recommended to directly specify the maximum bore bottom fillet on the drawing, or note a constraint such as "bore bottom fillet R ≤ 0.4." In materials with pronounced work hardening (such as stainless steel and titanium alloys), an overly small bore bottom fillet can also cause the boring tool to bite in the corner and produce chatter marks.

Face chamfers and relief grooves: assembly guidance and tool clearance

Chamfers at the entry of outer diameters and holes are not just for appearance; they serve as assembly guidance—especially during interference fits or blind assembly, a chamfer prevents damage on the first thread or first turn. Relief grooves are used during grinding or turning to give the grinding wheel or tool exit space at the end of the stroke. If the shape is non-compliant, subsequent operations are stuck. Once these two types of features are turned into specific dimensions on the drawing, the machinist knows whether to use a form tool or a standard tool.

A common rule: undercuts, thread runout, bore bottom fillets, chamfers, and relief grooves are not isolated dimensions; they are tied to the interference relationship with the mating part. When reviewing a drawing, first place the mating part beside it and walk through the assembly path—where it will contact first, where clearance is needed—then go back and specify dimensions. Specifying only the body dimensions without considering mating is the main reason these details are lost.

Material, tolerance, and surface roughness: three constraints on CNC turning feasibility

For the same drawing, changing the material, tolerance band, or roughness requirement will cause quotes and yield to diverge noticeably. These three are not parallel parameters but mutually constraining constraints: material determines how chips break and how long the tool can cut; tolerance band determines whether finish turning or grinding is needed; and roughness is often the item written overly tight out of habit and most likely to be questioned. To judge whether CNC turning can do it and whether it is worth doing, first look at the three separately.

Material determines chip form and tool life

Free-machining steel (such as 12L14 and 1215 types) turns most smoothly, with short, easily broken chips that do not tangle around the tool, and surfaces are easy to make fine; ordinary carbon steel and alloy steel are slightly stickier and require suitable speed and feed to break the chips. Stainless steel is another category: 304/316 work-harden noticeably. With too small a depth of cut, the tool rubs on the hardened layer, the tool tip wears quickly, the surface looks bright but dimensions begin to drift. Common industry practice is to maintain sufficient feed per revolution so the tool tip cuts below the hardened layer rather than lightly rubbing.

Aluminum alloys (6061, 7075) turn quickly and easily, but tend to stick to the tool and form built-up edge, which actually worsens the surface during finish turning; this is controlled with high speed, large rake angle, and cutting fluid. Brass chips are fragmented and break easily, making it a relatively worry-free material. Titanium alloys have poor thermal conductivity, concentrating heat at the tool tip, so cutting speed must be significantly reduced, otherwise the tool burns. Engineering plastics (POM, PEEK, nylon) have low cutting forces, but deform with slightly too much clamping force, and tend to burr and produce stringy chips that tangle. These differences are directly reflected in quotes—for the same features, changing material often has a greater impact than changing machines.

Tolerance band and roughness are two sides of one thing

Dimensional tolerance and surface roughness are highly coupled in turning. For conventional outer diameter turning, common industry achievable levels are IT8–IT9; to stably achieve IT7 or tighter usually requires finish turning, reduced depth of cut, controlled tool nose radius, or simply leaving grinding allowance. Roughness is similar: ordinary turning commonly achieves around Ra3.2, and under good conditions can reach Ra1.6; going further to Ra0.8 or Ra0.4 often requires finish turning, grinding, or rolling, with different costs and process routes.

Therefore, specifying Ra1.6 on non-mating surfaces on a drawing is often just habit, not a functional requirement. Relaxing an exposed but non-contacting surface from Ra1.6 to Ra3.2 often eliminates a finish turning or polishing step with no effect on assembly. What truly should be tightened are mating surfaces, sealing surfaces, and sliding surfaces. The way to judge is simple: ask "what does this surface contact, and what ensures the fit?" If there is no answer, the roughness can most likely be relaxed.

Comparison of chips from different materials in CNC turning with a close-up of the tool tip condition — The same turning tool cutting different materials produces very different chip forms and tool tip wear—this is also why changing material often affects cost more than changing machines.

Length-to-diameter ratio, thin walls, and interrupted cutting: the three typical failure entry points of CNC turning

The dimensions on the drawing are all within spec, yet the machined part fails inspection. Most of the time it is not that the machine tool lacks accuracy, but that the part has hit one of the three failure entry points of CNC turning: excessive length-to-diameter ratio, too-thin wall thickness, or a non-continuous cutting process. What these three types of problems have in common is that they cannot be seen on the drawing; only when the workpiece is mounted on the chuck and the tool tip actually cuts in do they reveal themselves as dimensional drift, chatter marks, or edge chipping. Below, they are broken down in the order of failure symptom, cause, and countermeasure.

Excessive length-to-diameter ratio: tool deflection, taper, and dimensional drift

When turning a slender shaft, one end of the workpiece is held by the chuck while the other end is unsupported. The radial cutting force bends the workpiece, so the tool tip actually cuts shallower than set, resulting in a barrel shape that is large in the middle and small at both ends, or a continuous taper from the clamped end to the free end. In terms of symptoms, if you measure the diameter at intervals along the same shaft and the values change monotonically rather than jumping randomly, it can basically be judged as tool deflection rather than tool wear. A common empirical threshold in the industry is to be on guard when the length-to-diameter ratio (overhang length ÷ diameter) exceeds 4:1, and above 8:1 a steady rest or follower rest is usually required; this number varies with material rigidity, tool lead angle, and radial depth of cut, so confirm it against the drawing and the actual fixturing plan. There are three directions for countermeasures: use a tailstock center or follower rest to support the free end; reduce the radial depth of cut and take more passes to bring the cutting force down; separate roughing and finishing, leaving stock in roughing and taking light cuts in finishing, so that the final dimensions are formed under low load.

Thin-walled parts: where clamping deformation and chatter marks come from

For thin-walled cylindrical parts or thin-walled sleeve-type parts, failure often occurs before cutting—as soon as the three-jaw chuck tightens, the workpiece has already been squeezed into a triangular round or an ellipse. After release it springs back elastically, but residual deformation and roundness error have already been left on the part. During machining, another layer of problems is superimposed: thin walls have low rigidity and are naturally close to the chatter-sensitive zone, so if the speed is slightly off, regular chatter marks appear and surface roughness drops a grade immediately.

Schematic of deformation when a thin-walled cylindrical part is held by a three-jaw chuck, comparing the clamped state with the roundness deviation after release

The core of the countermeasure is to change the clamping force from radial to axial or uniformly distributed: use soft jaws to increase the contact area, use a collet or split sleeve instead of three jaws, use face driving or a mandrel for locating from the bore, and if necessary first make a process boss so that clamping occurs on the stock, then cut it off before finishing. On the chatter side, suppress it by reducing the radial depth of cut, raising or lowering the speed to avoid the chatter zone, shortening the overhang, and choosing a sharper tool nose radius.

Interrupted cutting: tool tip life and dimensional consistency under impact load

Shafts with keyways, sleeves with cross holes, and eccentric stock on castings or forgings all cause the tool tip to experience an "entry—exit" impact on every revolution. The symptoms are tool tip chipping, abnormal flank wear, and dimensions slowly drifting within a few dozen parts. The damage of interrupted cutting to CNC turning is concentrated in two points: the impact force makes both the workpiece and the tool holder yield, worsening dimensional consistency; and thermal cycling causes microcracks in the tool tip carbide. Feasible directions are to choose a tougher grade and a larger tool nose radius, appropriately reduce speed and feed, place the depth of cut in a range with less impact, and if necessary first perform stress relief or pre-machining to flatten the interrupted surface before finishing.

These three failure entry points often appear at the same time: a slender thin-walled shaft simultaneously has a large length-to-diameter ratio and interrupted cutting, and the countermeasures can also constrain each other. Marking them out at the drawing review stage is much cheaper than trial and error on the machine.

Before quoting CNC turning, what should be confirmed first on the drawing

For the same rotational part drawing, getting quotes from different shops can differ by a large margin, often not because of the unit price but because of different fixturing plans. A part that can be completed in one setup versus one that must be turned around, mounted on a mandrel, or fitted with a steady rest differs in labor time in the auxiliary time. So the order of drawing review should be reasoned backward from the process chain, not starting with the material unit price.

First determine the datum and fixturing: the primary datum surface, clamping length, and whether there is a cylindrical section available for clamping. If the entire outer diameter of the part is a mating surface with no clamping position, then soft jaws, a mandrel, or face driving must be considered, and these will change the quotation structure. Then look at which dimensions the key tolerance zones fall on—coaxiality, face perpendicularity, and the fit tolerance between the bore and shaft determine whether finishing stock or grinding is needed.

Next confirm the details that are easily overlooked: the width and depth of the relief groove on the outer diameter and bore, the thread runout length, the fillet at the bottom of the bore, and the undercut. When these callouts are missing, the machinist can only use empirical values, and during assembly the parts may bottom out or the thread may not tighten all the way, with rework costs far higher than the time saved by omitting the callouts.

Finally confirm the material condition and subsequent processes: whether the stock is bar or forging, whether quenching and tempering or hardening is required, whether surface treatment is anodizing or plating, and whether inspection is full or sampling. Heat treatment changes dimensions, so grinding stock is often needed; surface treatment changes mating dimensions, so allowance must be reserved for threads and holes.

Only when these are listed clearly can quotes be comparable. A common situation in the industry is that when the length-to-diameter ratio exceeds 3 times, the wall thickness is less than one-tenth of the outer diameter, or the material is stainless steel or titanium alloy, the cost rises noticeably, and the specific multiplier still needs to be confirmed according to machine condition and batch size. If the drawing does not carry this information, the supplier can only quote the most conservative plan, and you lose the baseline for price comparison.

Frequently asked questions

The questions below all come from the specific judgment points in the previous text: fixturing datum, relief groove callouts, the trade-off between tolerance and roughness, and the failure entry points of length-to-diameter ratio and thin walls. The answers give criteria you can check against, not guaranteed values.

For the same rotational part drawing, why do quotes differ so much when the fixturing method changes?

Because the number of setups directly determines labor time and inspection fixtures. One setup can turn the outer diameter, face, and bore at the same time, and coaxiality is guaranteed by the machine itself; turning the other end after flipping requires re-alignment, and coaxiality becomes the superposition of two datums, often requiring an additional dial indicator or soft jaw turning operation. The quote difference mainly comes from the number of setups, whether a mandrel or steady rest is needed, and the accompanying increase in inspection actions, not simply the material cost.

If relief grooves and thread runout are not called out, can the machinist decide them himself?

He can, but what he decides are his habitual values, which may not match your mating part. The relief groove width, depth, and thread runout length determine whether the thread can be tightened all the way and whether it will bottom out during assembly. It is recommended to call out the groove width, groove bottom fillet, and runout form on the drawing (for example, runout per GB/T 3), and to review them together with the interference relationship of the mating part. Not calling them out is equivalent to leaving reproducibility to luck.

If the surface roughness of non-mating surfaces is relaxed from Ra1.6 to Ra3.2, can it really save cost?

Usually yes. Finer roughness often means smaller feed and lighter depth of cut, and sometimes requires a tool change or an additional finishing or grinding operation, which increases labor time and tool consumption. The premise is that the surface truly does not participate in fitting, sealing, or sliding. The way to judge is to see whether it has a fit tolerance, whether it contacts a seal ring or O-ring, and whether there is an appearance requirement. A common industry practice is Ra0.8–1.6 for mating surfaces and Ra3.2–6.3 for non-mating surfaces, subject to confirmation against the drawing and actual machining.

At what length-to-diameter ratio should a follower rest or steady rest be considered?

There is no one-size-fits-all number. Common industry experience is that after the length-to-diameter ratio exceeds 4–5 times, tool deflection and taper begin to become obvious, and above 8–10 times a follower rest, steady rest, or tailstock center is usually needed for support. The real criterion is the part rigidity, the material cutting force, and the tolerance zone you require: at the same length-to-diameter ratio, an aluminum alloy slender shaft and a stainless steel slender shaft behave completely differently. It is recommended to call out the tolerances and datums of the critical sections on the drawing and let the process side decide the support plan.

If a thin-walled cylindrical part drifts dimensionally after turning, is it a machine problem or a process problem?

In most cases it is the combined effect of clamping deformation and cutting heat. Radial clamping by a three-jaw chuck makes a thin-walled part become round in the clamped state and spring back after release, so the result differs depending on when you measure. Common countermeasures are to switch to soft jaws, increase the contact area, reduce clamping force, or change to axial clamping; at the same time control cutting heat and separate roughing and finishing. If the drawing allows, you can also leave stock, release the clamp, and then finish turn. This type of problem needs to be confirmed together with the process side regarding the measurement state and datum.

CNC Turning: From Workholding to Thread Relief Grooves, How a Revolved-Body Drawing Gets Made