A custom CNC shaft drawing has to settle three things: which diameters locate the part, which surface the inspector measures from, and how tight everything else really needs to be. Get those three right and the rest is detail. Get them wrong and the quote comes back padded, or the first article comes back wrong.
We see both every week.
A shaft is not a difficult part to draw. It is a difficult part to draw usefully, because the sheet has to survive three different readers: the estimator who prices it, the machinist who sets it up, and the inspector who signs it off. If any one of them has to guess, the guess becomes money.
The three places where shafts go wrong
Bearing seats. The shoulder face behind a bearing seat. And the point where a thread runs out into a plain diameter.
Those three account for most of the clarification emails we send. Not the exotic features. The ordinary ones.
Why they fail is different in each case. A seat diameter a couple of hundredths too generous lets the inner ring creep, and creep frets the surface, and fretting shows up as noise eighteen months later. A shoulder face that is square but has no relief leaves the bearing ring sitting on the tool nose radius instead of on the face. The part assembles. It also runs with a wobble nobody can explain. A thread cut straight into a shoulder cannot reach full depth on its last turn, so the nut stops short, and the gap was never on anyone’s drawing.
None of that is exotic. All of it is cheap to fix before the steel is cut.
Start with one sentence about the job
A shaft that carries torque and a shaft that guides a slide have almost nothing in common once you start putting numbers on them. The first lives or dies on the fits at its seats. The second lives or dies on straightness and surface condition along its travel. Tolerance both the same way and you waste money on one and take risk on the other.
So before the geometry is frozen, write one sentence. Something like: carries a 6202 bearing at each end, drives a pulley through a keyed section, sees about 3,000 rpm continuous.
That sentence does more work than a page of dimensions. It tells the machinist why the two seats are tight and the middle is not. It tells the estimator whether to plan a grinding operation. And when somebody in the chain asks whether the 12 mm section really needs to hold 0.01 mm, the sentence answers it without a meeting.
We ask for it on every RFQ. Some buyers think it is an odd request. The ones who have been through a failed first article usually send it without being asked the second time.
Pick datums an inspector can actually touch
Most drawing arguments we get into are not about tolerance values. They are about which surface the values are measured from.
Put five dimensions in a row, each with its own plus or minus, and the last feature in the row is no longer controlled to anything like the figure printed on it. The errors stack. If two bearing seats have to sit at a fixed distance because the housing is fixed, dimension that distance seat face to seat face. Directly. Not through three intermediate shoulders that happen to add up.
Same logic for the axis. A datum on one seat, a second datum on the other if the part is long, runout referenced to the pair. An inspector with a bench centre and a dial indicator can verify that in minutes. Ask the same inspector to chase a chain of stacked dimensions and he will ask for a CMM, and the CMM time lands on your invoice.
One detail worth stating on long parts. Past roughly ten times diameter, how you hold the shaft changes what the indicator reads. Between centres and in a chuck are two different measurements. If the function depends on it, say which condition applies.
Seats are fits, not tolerances
A seat diameter is not an abstract number. It is half of a fit on a precision bearing shaft, and the other half is the bearing you already chose.
Take the 6202 again, 15 mm bore. Light interference for a rotating inner ring sits somewhere in the j5 to k5 region of ISO 286. Turn the same position to h9 and it will slide on, feel fine in the hand, and creep under load. You do not have to write j5 on the drawing if you describe the fit in words. But the intent has to be unambiguous.
| Feature | Control this | Skip it and |
|---|---|---|
| Bearing seat | Diameter fit, roundness, Ra, shoulder squareness | Ring creeps, frets, or will not press on |
| Sliding section | Clearance, straightness, surface condition | Stick-slip, seal wear, uneven stroke |
| Press-fit section | Interference range, material condition | Mating bore cracks under hoop stress |
| Threaded end | Thread class, usable length, runout to seat | Nut binds, joint loses clamp load |
Two habits that save trouble.
- Name the mating part. On the drawing if you can, in the RFQ at minimum. “Bearing 6202, press fit” is worth ten times “tight”.
- Do not stack geometric controls on a seat that already has a tight size tolerance and a fine finish. Position plus concentricity plus runout on one diameter tells the shop the designer was unsure. Unsure drawings get priced defensively.
That corner at the base of a shoulder
Every stepped shaft has one, and almost none of them can be machined as drawn.
A turning tool has a nose radius. Draw a sharp internal corner and a radius arrives anyway, and whatever gets pushed against that shoulder sits on the radius instead of the face. The gap is a few hundredths of a millimetre. It is also enough to shift everything downstream axially.
Two honest answers. Specify an undercut, a narrow relief at the base of the shoulder, so the mating part reaches the face. Or specify the corner radius and accept that the mating part needs its own chamfer to clear it. What does not work is leaving the corner undefined and hoping the shop picks the version you had in mind.
Grinding changes the arithmetic. Grind a seat after hardening and the wheel needs somewhere to exit. A relief groove at the shoulder saves the wheel edge and protects the face it grinds up to. On hardened shafts we usually raise this before quoting, because adding a groove after the drawing is released means re-drawing, re-fixturing, and often a fresh setup charge that nobody budgeted.
Cross holes and flats cost setups, not just features
A shaft that only needs turning is a straightforward job. Add a cross hole at a defined angle, a flat that must clock to it, and a keyway, and now the part needs either live tooling with a C-axis or a second operation on a mill.
Both routes are legitimate CNC machining services. They do not cost the same, and the drawing should not pick the expensive one by accident.
Three things help.
- State the angular relationship, not only the position. “Hole 3 mm through, 25 mm from the left face” puts the hole in the right place along the axis and says nothing about where it points. If a flat or a keyway has to line up, dimension the angle from a named reference.
- Say whether the features are simultaneous. Two cross holes on one axis are easy. Two that must intersect at 90 degrees inside a small positional tolerance are a fixturing problem, and the quote will show it.
- Specify the thread properly. Designation, class, direction, usable length. “M8” alone leaves us assuming 6g and a length you did not intend. Plated threads shrink afterwards, which is its own paragraph.
Finish only where the surface works
Ra values get sprinkled across drawings because they look rigorous. They earn their place only where a surface functions.
A ground seat at Ra 0.4 µm and a turned clearance diameter at Ra 3.2 µm behave nothing alike, and the price gap between them is real. A lip seal needs a finish fine enough to protect the lip and not so fine that no oil film survives, which is a different question from hardness and a different question again from the lead of the turning marks.
That last point catches people. Turning marks run helically. Under a lip seal, a helix can pump fluid along the shaft, one direction or the other depending on rotation. On a sliding surface it steers wear. An Ra number does not describe direction. If direction matters, write it down.
Geometric tolerances that pay for themselves
Runout, concentricity, cylindricity, perpendicularity. All four describe real behaviour. All four cost money to verify. Three rules keep them honest.
- Tie the control to a function. Runout between two seats controls the orbit of the assembled shaft. That matters on a rotating part. On a static locating pin it mostly does not.
- Use total runout when you mean the whole surface. Circular runout samples one revolution at each station. Total runout covers the surface and picks up taper and axis error, which is closer to what a bearing actually feels.
- Do not stack controls that describe the same deviation. Three callouts on one diameter produce a drawing no inspector can satisfy economically, and a shop that prices the worst reading of all three.
Heat treatment and coating move the size you drew
Specify a case depth, a hardness and a zinc-nickel coating, and forget to say which dimension is measured before plating, and you will get parts that fail final gauge while being dimensionally correct.
Plating builds on every surface, thread flanks and seat diameters included. On a tight fit that build-up is not a rounding error. Two conventional answers: dimension the critical diameter before coating and keep the coating thin and controlled, or mask the functional surfaces so nothing lands on them.
Heat treatment has its own constraints. Distortion after quench is normal, which is why a hardened steel shaft is usually roughed, treated, then ground. If the drawing asks for a hard seat and a fine finish, the route needs a grinding allowance, and the tolerance has to be achievable after grinding rather than before it.
For high-strength plated parts, hydrogen embrittlement is a risk rather than a footnote. Baking after plating is standard practice for us, and the requirement belongs on the drawing so nobody compresses it out of the production schedule. The same reasoning applies to inspection: hardness, tensile, salt spray and coating thickness checks are only meaningful if the drawing states the acceptance limit they are being measured against.
What we want in the RFQ
Two files, not five. A 2D drawing with tolerances and a 3D model for geometry. The drawing governs. The model settles blends and transitions that a printed sheet handles badly.
Then the things that never fit a title block: material and condition, hardness if it matters, coating and where it is permitted, the critical dimensions and what each one does, annual quantity next to prototype quantity, and whether you need a first article report or a full dimensional report with the shipment.
That last item moves the price more than most buyers expect. A hundred-piece order with a full report can cost more per part than a thousand pieces without one, because a report is labour, not material.
Quantity also picks the process. Turning on our equipment is quoted to 0.006 mm where the drawing and the process justify it, across twenty lathes that run prototypes and production on the same floor. Whether your part needs that is a separate conversation, and a cheaper one to have before the order.
If you want to see the lathes and the lab behind those numbers, our manufacturing and inspection capability page lists both.
Four mistakes we see over and over
- Tolerancing every dimension to the same figure. It reads as thorough. It actually tells the shop that nothing was prioritised, so the shop prices the tightest case across the whole part.
- Writing “high precision” or “as per sample” where a number belongs. A sample records what one part measured on one afternoon. It is not an acceptance limit.
- Leaving material condition off. 304 in the annealed state and 304 cold-worked machine differently, and one of them keeps moving after the cut.
- Skipping the angular reference for cross features, then rejecting the first article because the flat points the wrong way. We have seen that rejection three times this year, and it costs a fortnight every time.
FAQ
Do I need a 3D model as well as a 2D drawing?
It helps, particularly for blended transitions and milled features. It does not replace the drawing. Tolerances, datums and notes need a home, and that home is the 2D sheet.
What tolerance can CNC turning actually hold?
Depends on diameter, length, material and how the part is held. A short stiff 303 part can be held very tight. A long slender aluminium shaft deflects under its own cutting force and no amount of machine accuracy fixes that. Ask for what the function needs, then let the shop tell you whether the process supports it.
Should the seat tolerance follow the bearing or the housing?
The bearing, and whether the ring rotates. Rotating inner ring needs interference. A stationary inner ring on a rotating shaft can take a transition fit. The housing fit is a separate decision and should not drive the shaft callout.
Is an undercut always necessary at a shoulder?
No. It is necessary when the mating part must seat flat and has no chamfer of its own, or when a grinding wheel needs clearance. Where the mating part is chamfered and axial position is not critical, a defined corner radius is enough.
How do I add a coating without losing the fit?
State the finished dimension on the functional surface and say whether it is measured before or after coating. If coating thickness cannot be held tightly enough, mask the surface. This one ambiguity causes more out-of-tolerance shafts than any other, and the parts are usually dimensionally correct when they fail.
A drawing is a manufacturing instruction, not a record of design intent. They overlap, but they are different documents. When the seats, the datums and the critical dimensions are clear, a shop can plan a process, quote honestly, and inspect against something measurable. When they are vague, the gaps get filled with assumptions, and assumptions are what come back in the first article report.
Click Here To Get Wholesale Quotation | Free SamplesPost time: Nov-14-2026