Guides / Process

Design for Swiss Machining: Drawing Choices That Move the Price

September 20, 2026

A Swiss machining quote is decided mostly on your drawing, not on which shop you send it to. The same part sent to three shops that run Swiss-type lathes usually comes back within a fairly narrow band. Change the drawing, and the price moves further than shopping around ever will.

This guide covers the design choices that matter most on a sliding headstock lathe, in the order they affect a quote. It assumes you already know how Swiss-type turning works.

Start with length to diameter

The length to diameter ratio, written L/D, decides whether a Swiss machine is the right process at all. It is the machined length of a feature divided by its diameter.

Under about 3:1, most conventional CNC lathes hold the part fine and a Swiss machine offers no advantage on rigidity. From roughly 3:1 up to 20:1 and beyond, the guide bushing carries the part right next to the cut and the Swiss machine pulls clearly ahead. A 4 mm diameter shaft 60 mm long is a 15:1 part, and it will come off a Swiss lathe straighter than off a conventional lathe with a tailstock.

What this means for your drawing:

• If the part is short and fat, expect a shop to say a conventional lathe quotes lower. That is a fair answer.
• If the part is slender, say so on the RFQ. It is the single trait that points a request at the right machine.
• Do not add length that has no function. Every extra millimeter is bar cost and cycle time.

Keep the largest diameter down

Everything on a Swiss part starts as round bar, and the bar has to be at least as large as the biggest diameter on the print. That one number drives three costs at once.

First, bar price. A part with a 12 mm head and a 4 mm body runs from 12 mm bar, and the 8 mm difference turns into chips along the whole body length. Second, machine choice. Bar capacity is usually around 20, 32 or 38 mm, so a large flange can push the job onto a bigger machine with a higher hourly rate, or off Swiss entirely. Third, cycle time, because removing that material takes passes.

If a head or flange exists only to give a wrench flat or a stop face, ask whether a smaller hex or a shoulder would do the same job. Cutting the largest diameter by a few millimeters often saves more than any other single change.

Design around standard tools

A Swiss machine carries a fixed set of tools loaded at setup, typically 10 to 20 positions. Every tool you force the shop to grind specially adds setup hours and a lead time risk if it wears out mid run.

Features that use stock tooling:

• Drill diameters in common increments rather than an odd size that only your model needs
• Standard thread forms and pitches, metric or unified
• Groove widths that match a standard parting or grooving insert
• Chamfers at 45 degrees, or at the angle your other parts already use
• Corner radii that match a standard insert nose radius

A common example: an O-ring groove drawn at 1.15 mm wide because that is what the CAD library produced. Widening it to a standard insert width changes nothing about sealing and removes a ground tool from the setup.

Threads

Threads are where drawings quietly add cost. Three choices matter.

Form and pitch. A standard coarse pitch in a common size runs on a stock insert or die head. A fine pitch in an unusual size may need a special tool.

Thread relief. A thread that must run fully up to a shoulder needs a relief groove or a special approach. If the mating part does not require full thread to the shoulder, allow an incomplete first thread and say so in a note.

Cut, rolled or whirled. Cutting is the default and suits most parts. Thread whirling produces a strong, clean thread on long slender parts such as bone screws, but not every shop has the attachment, so it narrows your supplier list. Say which you need only if the application actually requires it.

Also state the thread class or fit. A shop that does not know whether you need a free fit or a close fit will assume the tighter one and gauge accordingly.

Cross holes, flats and slots

Live tools are what let a Swiss part come off finished. A driven spindle in the gang can drill a cross hole, mill a flat, cut a slot or broach a hex while the main spindle holds position.

Good practice:

• Put cross holes on one plane when you can. Several holes at odd angles each need their own index and, sometimes, their own tool.
• Keep cross holes away from the very end of a slender section, where the drill can push the part.
• Make flats wide enough for a standard end mill to clear in one or two passes.
• A hex or square broached in one shot is usually cheaper than milling the same shape with multiple passes.

Every driven operation adds seconds, and on a part running 50,000 pieces a year, seconds are real money. The cost guide shows how cycle time translates into part price at volume.

Back end features

The sub spindle picks up the part after cut off and machines the back. This is nearly free compared with a second operation on another machine, but only within limits.

Things that work well on the back end: a chamfer, a center drill, a short drilled or tapped hole, a face groove, a shallow pocket, a back turn. Things that struggle: deep drilling, heavy milling, features needing high precision relative to a front end feature on the same axis.

Where a diameter on the front and a bore on the back must stay concentric within a few microns, flag it. The shop may hold the part differently or add a check. Silence on the drawing leads to surprises at first article.

What to avoid

These five features raise a quote more than they look like they should:

1. Deep small holes. A hole deeper than about 10 times its diameter needs pecking, a gun drill or a special cycle. The deeper it goes, the slower it gets.
2. Sharp internal corners. A turning tool leaves a radius. Demanding a sharp corner means a second tool or a grinding operation.
3. Thin walls on a tube. A wall under about 0.5 mm flexes under the tool and under gauging pressure, and parts spring out of tolerance after cut off.
4. Undercuts that need a form tool. If the profile cannot be reached by a standard insert path, someone has to grind a tool for it.
5. Full length tight diameter. A diameter held to a few microns over 40 mm of length is far harder than the same tolerance over 5 mm. State where on the length it applies.

None of these are impossible. They just need to be worth their cost.

Tolerance only what matters

Swiss machines hold tight diameters well. Typical diameter tolerances on free machining materials land around ±0.005 to ±0.013 mm on a good machine, but every tolerance tighter than the shop’s normal practice adds finishing passes, in-process gauging and slower inspection.

The rule that saves the most money: mark the two or three features that control function, and let a sensible general tolerance block cover the rest. A print with ±0.005 mm on one bearing diameter and ±0.05 mm elsewhere quotes far lower than the same part with ±0.005 mm everywhere, and the parts work the same. For how these numbers behave in practice, see the guide to Swiss machining tolerances.

The same applies to geometric callouts. Concentricity between diameters cut in one chucking is largely free, because they are cut on one axis. Concentricity between a front feature and a back feature is not.

Surface finish

Surface finish is specified more often than it is needed. A turned finish around Ra 0.8 to 1.6 µm is typical straight off a Swiss lathe with normal parameters. Asking for Ra 0.4 µm or better means slower finishing passes, sharper tooling changed more often, sometimes a polishing step.

Call out finish on sealing surfaces, sliding surfaces and anything that mates with an O-ring. Leave the rest at the general note. Where a finish is cosmetic rather than functional, write that down, because it changes how the shop inspects it.

A quick substitution table

Drawn as	Often cheaper as	Why
Odd drill diameter	Nearest standard size	Stock tool, no grind
Narrow custom groove	Standard insert width	Stock tool, faster
Sharp internal corner	Corner with insert radius	One tool instead of two
Fine pitch special thread	Standard coarse pitch	Stock insert or die
Tolerance everywhere	Tolerance on 2 or 3 features	Fewer finish passes, less gauging
Ra 0.4 µm overall	Ra 0.8 to 1.6 µm, tight only where it seals	Normal parameters, fewer tool changes
Large head on slender body	Smaller head or shoulder	Smaller bar, less material removed

Numbers here are typical starting points. A shop quoting your specific part may reach a different conclusion, and a good one will explain why.

Before you send the drawing

Run this short check:

1. Is the largest diameter as small as function allows?
2. Are drill sizes, thread pitches and groove widths standard?
3. Is every tolerance tighter than the general block there for a reason?
4. Does any surface finish callout have a function behind it?
5. Are cross holes grouped on as few planes as possible?
6. Have you stated which features are critical, and why?
7. Have you given the yearly volume, not just the first order?

Send the STEP file, the PDF drawing and those answers through the RFQ form. We match the part with up to three shops that run Swiss-type lathes and reply within 24 business hours. If the part would be cheaper on a conventional lathe, we will say so.

Frequently asked questions

Keep reading

• Guide Bushing vs Guide Bushing-Less Swiss Turning
• Swiss Machining Services: How Swiss-Type Turning Works and What It Is Good For