Design for machining

Q: What is the minimum wall thickness for CNC machining?

A published Protolabs Network starting point is 0.8 mm for metals and 1.5 mm for plastics. Wall height, unsupported span, material, finish and fixturing can require thicker sections. These figures are design guidance, not a universal minimum or a FabDigit acceptance limit.

Q: Why can’t a milled pocket have a perfectly sharp internal corner?

A rotating end mill leaves an internal radius. Increase the radius, add a relief for the mating corner, or assess another operation. Wire EDM needs an accessible through-cut path and an electrically conductive material; it cannot make every blind-pocket corner.

Q: How deep can a pocket be?

Depth depends on the finishing cutter, its reach and holder clearance. Common end mills often have cutting lengths around 3–4 diameters, but specialized tools can go deeper. A 24 mm-deep pocket with R2 corners implies at least a 6:1 depth-to-diameter ratio for the corner tool; opening the corners may reduce that ratio.

Q: What tolerance can CNC machining hold?

The achievable and economical tolerance depends on feature size, geometry, material, process and inspection. Define the fit or datum relationship required by the assembly and have it confirmed for the quoted part. A machine accuracy specification or one supplier’s standard is not a universal part tolerance.

Q: How much do tight tolerances add to the price?

There is no fixed percentage. They may require more stable stock, an extra finishing operation, controlled inspection or a dedicated fixture. Compare the same CAD at the required critical-feature tolerances and a relaxed nonfunctional specification to find the actual cost driver.

Q: Should I model threads?

For ordinary threads, a plain pilot hole plus a drawing callout for system, size, pitch, class and full thread depth is usually clearer. Show special thread forms explicitly. Check screw engagement independently from the drilled depth and the tool runout.

Q: When is 5-axis cheaper than 3-axis?

It can be cheaper when reduced re-clamping, shorter tool reach or better access saves more time than the added machine and programming cost. Simple accessible geometry may favor 3-axis. Five-axis access still needs suitable workholding and holder clearance.

Q: What files do I upload for a CNC quote?

Provide the revision-matched solid model and a drawing for critical tolerances, threads, surface texture and finishing. Include material condition, quantity, the final state of dimensions and required inspection or material records.

Q: Should a machined dimension be specified before or after finishing?

Specify the state that meets the assembly requirement, usually the delivered condition. If a feature is masked or machined after coating, identify it. Added deposits reduce hole diameters by twice the per-wall buildup; anodize requires its actual outward-growth allowance, not twice its total oxide thickness.

Q: When should I use 3D printing instead of CNC machining?

Printing can suit enclosed geometry, consolidation and rapid changes. CNC can suit a required stock material, an accessible precision fit or a machined sealing surface. Compare the exact material, final finish, quantity and validation requirement rather than process names alone.

Design a part the cutter can reach, the fixture can hold and the inspector can measure. Practical choices for walls, pockets, holes, threads, datums and finished fits in milled and turned parts.

Updated September 2026 · Milling and turning · Geometry, fits and finishing

Get an instant quote CNC machining cost guide

Start with access, support and function

For a first design review, identify the assembly interfaces before reducing weight or adding detail. A small change at a deep corner can matter more than a large change to an open outside face.

Access

Can the tool reach every face?

Include the cutter, shank and holder in the clearance check. A visible surface is not necessarily reachable with a tool stiff enough to finish it.

Support

What holds the part during the last cut?

Leave a practical gripping surface or discuss sacrificial stock and soft jaws. A thin finished shell may need more support than its starting billet.

Function

Which dimensions make the assembly work?

Separate locating holes, bearing seats and sealing surfaces from cosmetic boundaries. Give each critical feature a final-condition requirement and a measurement reference.

Sequence

What happens after machining?

Heat treatment, coating and removal from the fixture can change the result. Plan the sequence around the delivered fit rather than the first machined size.

Wall thickness, corner radii and pocket floors

There is no universal minimum wall. Height, unsupported span, material and the direction of cutting forces decide whether a thin feature stays stable.

The cutter and its holder define the usable space

The corner limits the cutter

In this plan view, a pocket with a larger internal radius admits a larger cutter. Give the cutter room to arc around the corner; a relief can clear a square mating part.

The holder also needs clearance

In section, a long tool must clear the pocket mouth with its shank and holder. A shorter reach reduces deflection; changing the corner alone may not clear the holder.

Schematic views, not to scale. The manufacturing plan must match the part geometry and material.

Early DFM checks — starting points, not acceptance limits
Feature	Useful starting point	What to check
Metal walls	Protolabs Network recommends 0.8 mm; increase thickness for tall or broad walls	That published minimum does not establish stiffness, flatness or FabDigit capability for your part
Plastic walls	The same guide recommends 1.5 mm	Allow for lower stiffness, cutting heat and stress release; specify the polymer and condition
Internal vertical corners	Use the largest radius the mating geometry allows	A radius slightly larger than the chosen cutter radius permits an arc through the corner
Pocket floor	Keep a supported section below the pocket	A thin floor can deflect during machining or bow after unclamping; add ribs or change the machining sequence
Wall-to-floor transition	State whether a fillet is functional	An end mill may have a corner radius; a ball tool is not required for every floor fillet
Small bosses and ribs	Review their height as well as their width	Tool clearance around the feature and support during deburring can govern feasibility

The wall figures are published supplier guidance, not an industry standard. A feasible thin feature may still need a different tolerance or fixture from the surrounding part.

Use relief where a square part must fit. A local dog-bone or T-bone can clear a sharp mating corner without making every pocket corner tiny. Check that the relief does not cut into a sealing land or a highly stressed section.
Avoid unnecessary full-round edges. A specified chamfer may be easier to produce and inspect than a continuous cosmetic radius. Define the edge break so it cannot consume a thin lip.

Pocket depth is a tool-reach decision

A broad pocket can still be difficult if its last corner needs a small cutter. Separate bulk roughing from the tool that must finish the deepest detail.

Worked geometry check: a 24 mm-deep pocket with an R2 corner admits a cutter no larger than Ø4 mm at that corner. The depth-to-diameter ratio is at least 6:1, before clearance below the holder. Changing the corner to R4 could admit a cutter near Ø8 mm and bring that ratio toward 3:1. The functional corner and actual tool selection decide whether this change is acceptable.

What makes a deep feature expensive
Design condition	Better question	Possible change
Deep pocket with tight corners	What is the reach-to-diameter ratio of the finishing tool?	Open only the nonfunctional corners, shorten the deep region or allow corner relief
Long narrow slot	Can chips escape without recutting and can the tool enter?	Open an end, reduce the depth or discuss a different toolpath
T-slot or internal undercut	Can the cutter head enter and can the neck clear the wall?	Match a catalog cutter geometry, move the undercut toward an opening or split the part
Hidden internal passage	Can it be drilled and plugged, or assembled from accessible parts?	Compare a split body with a sealed joint against additive manufacturing
Deep cosmetic cavity	Does the entire cavity need the same roughness?	Apply the finish requirement to the contact region rather than every inaccessible wall

Common end mills often have cutting lengths around 3–4 diameters. This is an economical design reference, not a hard reach limit: extended tools, relieved shanks and other strategies exist. Tilting a 5-axis tool does not halve the depth of a sealed pocket or remove holder collisions.

Separate hole depth, thread depth and screw engagement

These are three different dimensions. Specify the useful thread and the assembled engagement, then leave room for the selected tool and the drill point.

Hole and fastener details to resolve on the drawing
Feature	Specify	Design implication
Plain hole	Diameter, tolerance, through or blind, and depth reference	Standard drill sizes simplify tooling, but interpolation, boring and reaming are valid options for other diameters
Blind hole bottom	Whether the functional depth excludes the drill point	A conventional drill leaves a conical end; a required flat bottom changes tooling or adds an operation
Internal thread	Thread system, size, pitch, class and minimum full thread depth	Example: M4 × 0.7–6H, minimum 8 mm full thread; separately define the allowed drilled depth
Thread engagement	Screw length after washers, gaps and countersinks are included	Select engagement against internal-thread stripping and screw tensile strength; there is no depth after which all extra threads carry zero load
Insert	Exact insert and installation method	Wire inserts, solid inserts and self-clinching hardware need different holes and supporting geometry
Repeated assembly	Tightening method, torque, cycle requirement and access	An insert can improve durability in a soft substrate; aluminum threads do not automatically fail after a few uses
Counterbore or countersink	Head clearance, seating surface and minimum material beneath	Check the actual fastener standard and tool access instead of adding a generic depth allowance

Do not apply a universal three-pitch allowance. Tap lead, runout, chip space and the drill point vary by tool. State full thread depth and maximum hole depth; let the machining plan resolve the tool clearance.
Keep ordinary threads simple in CAD. A plain pilot hole with a complete drawing callout avoids unnecessary helical geometry. Supply detailed geometry for a nonstandard thread or special form, and flag it explicitly.
Treat deep holes separately. Straightness, coolant access, breakout and intersecting passages can matter more than the diameter alone. Identify an alignment-critical bore before choosing its process.

Datums and setups should follow the assembly

A setup changes how the part is held and referenced. Several faces may be reached in one indexed setup, but workholding and calibration error still exist.

3-axis

Accessible prismatic features

A plate or block with mostly orthogonal features may be economical with simple fixtures and a small number of flips. Identify which relationships must survive those flips.

3+2

Indexed access to several faces

The rotary axes position the part before cutting. This can reduce re-clamping while retaining a fixed cutting orientation for each feature.

5-axis

Continuous tool orientation

Simultaneous motion can suit sculpted surfaces or access that needs a changing tool angle. It still needs collision clearance and a fixture that leaves the required surfaces exposed.

Turn an assembly need into a measurable requirement
Assembly need	Drawing approach	Manufacturing question
A housing sits flat on a base	Identify the mounting face and its flatness/contact requirement	Is it measured free of clamps and after coating?
Two bores must locate one shaft	Control size and their relationship to a functional datum system	Can the bores be finished in the same setup, or line-bored?
A hole pattern locates a mating plate	Define datum features, pattern position and hole sizes	Is a functional gauge appropriate, or are coordinate measurements required?
A block is symmetric in CAD	Provide an orientation reference where assembly could be reversed	Can the operator and inspector distinguish the intended faces?

One setup can reduce relocation error. It does not guarantee any fixed tolerance for free; thermal drift, tool wear, workpiece movement and measurement uncertainty remain.

Turned parts need support at the cut

For shafts and bores, distinguish the slenderness of the workpiece from the overhang of the tool. They are separate sources of vibration and deflection.

Turning decisions for shafts, sleeves and housings
Feature	Plan for	Drawing detail
Long shaft	Tailstock, steady rest, guide bushing or a different sequence	Indicate whether center holes and temporary support surfaces are acceptable
Deep bore	The largest practical boring bar with the shortest overhang	Specify straightness, size, finish and a bottom relief only where needed
Thin sleeve	Controlled chuck force or a supporting mandrel	State whether roundness is required in the free state or installed state
Shoulder and bearing seat	Tool nose radius and mating-part chamfer clearance	Use a defined relief if a bearing must seat fully against the shoulder
Groove or external thread	Insert width, tool exit and inspection access	Name the groove or thread standard and its functional dimensions
Cross hole or flat	Live tooling or a secondary milling setup	Locate it from the turned datum when angular orientation matters

For internal thread turning, Sandvik Coromant gives different overhang guidance for steel, damped and carbide bars. The ratio uses bar diameter, not simply bore diameter; a generic “4× bore depth” rule misses this distinction.

Choose the grade and condition before optimizing the cut

A machinability comparison is useful after the material meets the operating environment. Stock form, heat treatment and residual stress also change the manufacturing route.

Go-to machining grades — machinability and relative cost
Material	Machinability	Weldability	Cost	Use it for
Aluminum 6061	Very good	Very good	$	General CNC machined parts; Aerospace and structural brackets; Hydraulic manifolds and valve bodies
Aluminum 7075	Excellent	Not recommended	$$$	Aerospace components; Defense equipment; Gears
Aluminum 2024	Excellent	Not recommended	$$$	Aircraft skins and fuselage panels; Wing and fuselage structural members; Aerospace fittings and brackets
Aluminum 6082	Very good	Very good	$$	Trusses; Bridges; Frames
Steel 1018	Very good	Excellent	$	Motor shafts; Tie rods; Machined pins, spacers and bushings
Steel 1045	Good	Good	$	Gears; Axles; Shafts
Steel 4140	Good	Good	$$	CNC machined gears; Transmission and drive shafts; Machine tool spindles
Steel 12L14	Excellent	Not recommended	$	Machined fittings; Fasteners; Valve bodies
Stainless Steel 303	Very good	Not recommended	$$$	CNC turned shafts; Valve bodies and stems; Nuts and threaded fittings
Stainless Steel 304	Fair	Excellent	$$	Food processing equipment; Kitchen appliances and sinks; Sanitary tanks and process piping
Stainless Steel 316	Fair	Excellent	$$$	Marine deck hardware and fasteners; Chemical process piping and tanks; Food and pharmaceutical processing equipment
Stainless Steel 17-4 PH	Fair	Very good	$$$	Pump shafts; Valve stems and internals; Aerospace structural fittings
Copper Alloy C36000	Excellent	Not recommended	$$$	CNC turned threaded parts and fasteners; Hydraulic and pneumatic fittings; Valve stems and valve cores
Copper Alloy C11000	Fair	Good	$$$$	Electrical busbars; Grounding straps and connectors; Terminals and cable lugs
Titanium Grade 5	Poor	Good	$$$	Aircraft turbine blades and engine hardware; Medical implants and instrument bodies; Airframe structural fittings and lugs
POM-C	Excellent	Good	$$	Chemical-resistant gears; Bearings and bushings; Slide plates and wear guides
PA6	Very good	Good	$	Automotive gears; Pulleys; Caster wheels
PC	Very good	Excellent	$	Machine guards and safety shields; Clear windows and glazing panels; Lighting lenses and light pipes
ABS	Excellent	Excellent	$	Electronic enclosures and housings; Power tool housings; Computer keyboards
PEEK	Very good	Very good	$$$$$	Spinal fusion implants; Aerospace seals and back-up rings; Downhole oil and gas seals
PTFE	Good	Not recommended	$$$	Seals; Gaskets; Liners
UHMW-PE	Fair	Poor	$$	Chute and hopper liners; Conveyor wear strips; Conveyor guide rails and curves

Machinability and weldability are the library’s 0–100 scores (Excellent ≥ 85 … Poor < 35); cost is the relative tier, not a price. Every grade links to its datasheet with tempers, heat treatments and the finishes it takes.

All CNC machining grades

Specify the delivered condition. 6061-T6, 4140 pre-hardened and 17-4 PH H900 describe different material states. If hardening follows rough machining, leave a route for distortion correction and final finishing.
Treat polymer movement by material. Nylon moisture conditioning can alter dimensions. PTFE has very different water uptake but can creep under load. POM, PEEK and acrylic each need their own temperature, stress and chemical assessment.
Avoid fixed cutting-speed ratios between alloys. The tool, operation, engagement, coolant and material condition determine usable settings. A grade that cuts more slowly can still be the right choice if it removes a later coating or heat-treatment step.
Compare finished geometry with available stock. Allow enough material for sawing, workholding and cleanup. A nominal stock dimension is not a guaranteed finished dimension; small dimensional changes can alter which blank is economical.

Specify the fit, then choose its tolerance

A tolerance is an acceptance requirement, not a machine specification. Its cost depends on the feature, span, material, process sequence and inspection method.

Worked fit example: a hole specified as 10.00–10.02 mm and a shaft specified as 9.96–9.98 mm have 0.02–0.06 mm diametral clearance. The calculation uses the smallest hole minus the largest shaft, then the largest hole minus the smallest shaft. These are illustrative drawing limits, not a stated process capability. For an interference joint, see the press-fit tolerance guide for the complete shaft/hole stack and assembly requirements.

Make each requirement do a specific job
Requirement	What it controls	What it does not establish
Diameter limits	The allowed size interval for a hole or shaft	Position, straightness or the fit against an unspecified mating part
Flatness	Form of a surface within a defined tolerance zone	Orientation to another surface
Position with datums	Location of a feature relative to the functional datum system	An interchangeable substitute for a ± size tolerance
Surface roughness	A specified texture parameter on the indicated surface	Flatness, waviness, sealing performance or leak tightness by itself
General tolerance standard	The unindividually toleranced features within its defined scope	One fixed ± value for every nominal size, angle and geometric characteristic

H7 alone does not define the fit. It defines a hole tolerance zone tied to nominal size. Pair it with the shaft requirement and check assembly force, operating temperature and lubricant needs.
Use a clear general note. If ISO 2768-1 class m is chosen, its linear tolerances vary with nominal dimension. Do not translate the entire standard into “±0.1 mm everywhere”; identify individual exceptions.
Compare quotes at the same inspection scope. A first-article report, selected-feature inspection and a full dimensional report answer different questions. Call out the characteristics that need recorded results.

Tightening an accessible small bore may require different work from tightening a broad thin plate. There is no universal percentage surcharge or a single tolerance guaranteed by all CNC processes.

Choose the surface for its job

Separate appearance, texture, wear, corrosion protection and electrical contact. One finish rarely satisfies all of them on every face.

Specify the important consequence, not only the finish name
Finish	Design decision	Confirm on the drawing
Machined surface	Set roughness where function needs it; tool marks elsewhere may be acceptable	Parameter and limit, indicated faces, and any lay direction that affects sealing or sliding
Bead blast	Texture and edge rounding depend on media and process	Cosmetic faces, mask boundaries and surfaces that must retain size or edge definition
Anodize	Oxide grows into aluminum and outward from its original surface	Type, coating thickness, seal, colour and final fit or masking requirement
Electroless nickel or other plating	An added deposit changes diameters and thread fits	Thickness range, underlayers if any, masking and inspection after plating
Black oxide	A thin conversion layer with performance affected by the supplementary seal or oil	Corrosion requirement and final dimensions; avoid treating it as outdoor protection by default
Paint or powder coat	Film build occupies clearance and needs accessible masking boundaries	Grounding points, threads, gasket lands, contact surfaces and final coating specification
Grinding after heat treatment	Final material removal can restore size or form after distortion	Grinding allowance, treated depth and which faces remain protected

Budget the fit after the finish

An uncoated part that assembles correctly can become an interference fit after treatment. Apply the allowance to each mating surface and include the coating thickness variation.

Both mating features contribute to the clearance

Design the mating pair

Clearance is the hole diameter minus the shaft diameter. Both parts contribute to the final fit.

Allow for the worst case

Minimum clearance = smallest hole − largest shaft. A nominal gap alone does not guarantee free movement.

Schematic illustrations; not to scale. Confirm the design for the chosen material, process and final use.

An added-coating example: assume the hole above receives a uniform deposit of 0.010 mm per side and the shaft stays uncoated. The finished hole becomes 9.98–10.00 mm, so its clearance against the 9.96–9.98 mm shaft becomes 0.00–0.04 mm. Coating variation could reduce that minimum further. Masking, pre-machining allowance or finishing after coating must be chosen before release.

Anodize uses a different allowance. Total oxide thickness is not all outward growth. The Aluminum Anodizers Council gives nominal outward-growth estimates of about one-third of total thickness for Type II and one-half for Type III; alloy, processing and pretreatment can change the result. If outward growth is 10 µm on each wall of a bore, its diameter decreases by about 20 µm; do not automatically use twice the total oxide thickness. For functional texture requirements, see surface roughness Ra and Rz.

Define the delivered state. State whether the dimension applies after heat treatment, coating and insert installation. A masked bore and a bore machined after anodizing have different exposed surfaces and corrosion consequences.
Include the actual mating part. Use its size limits and coating condition. For a press fit, also assess contact pressure, assembly method and the strength of the surrounding wall.

A release package the machinist and inspector can use

Keep the CAD, drawing and requested configuration on the same revision. Resolve conflicts before manufacturing rather than relying on an unstated order of precedence.

Geometry and revision. Send a solid model per part, assembly context where needed and a revision-matched drawing. Identify a handed part or an intentional mirror version.
Material and final condition. Name the alloy or polymer, temper or hardness, allowed substitutions and material certification needs.
Critical characteristics. Identify datum features, fit limits, thread specifications, sealing lands and free-state flatness. State which measured results must accompany delivery.
Finishing sequence. Include surface texture, coating thickness, masking and the stage at which dimensions apply. Indicate permitted witness marks and edge breaks.
Quantity and repeat orders. Give the initial batch and expected repeats. An initial fixture or inspection gauge may be worthwhile across the program even when it adds to the first order.

For pricing drivers, see the CNC machining cost guide. For route selection, compare CNC machining and 3D printing.