CNC Metal Cost Guide

• 1
  Key takeaways
• 2
  What moves the price, and by how much
• 3
  How to read a CNC metal cost breakdown
• 4
  Material choice: the cost you can see and the cost you cannot
• 5
  Geometry and tolerance: where cycle time is really spent
• 6
  3-axis, 4-axis or 5-axis: when the higher rate is cheaper
• 7
  Quantity, setup and the cost per part curve
• 8
  Finishing, inspection and the hidden add-ons
• 9
  How to compare CNC metal quotes step by step

Most metal machining quotes come back as one number. That number is built from six or seven smaller numbers, and knowing which ones are large tells you where to push back in a redesign. A useful CNC metal cost guide should let you look at a drawing and predict the direction of the price before the quote arrives.

Start with the stock. A part cut from a 60 × 60 × 120 mm aluminium block wastes a lot of material that never becomes a chip. When the design allows, a near-net shape from casting or extrusion cuts both material cost and roughing time. On titanium and Inconel, this matters far more than on 6061.

Then look at how many times the part is touched. Every new orientation means a new fixture, a new zero point and a new chance to lose alignment. A part that can be reached from three sides on a 5-axis machine is usually cheaper than the same part run on three separate 3-axis setups, even though the 5-axis hourly rate is higher.

Finally, separate the machining price from the finishing and inspection price. These are real costs, but they scale differently. Anodizing scales with surface area. CMM inspection scales with the number of tolerance callouts you marked as critical.

Material price per kilogram is the easy part. The harder part is the machinability, because it decides feed rate, tool wear and how often the operator stops to check the tool. Free-machining aluminium 6061 and brass C36000 cut fast and hold a good finish with little effort. Stainless 316 and 17-4PH work-harden if the feed is too light, so the programmer has to take a heavier cut than looks comfortable.

Titanium TC4 (Ti-6Al-4V) is a different problem. It conducts heat poorly, so most of the cutting heat goes into the tool edge instead of the chip. Tools wear faster, spindle speeds drop, and a feature that takes 8 minutes in aluminium may take 40 minutes in titanium. That is the real reason titanium parts cost more, not the bar price alone.

There is also the stock form. Plate, bar, tube and near-net casting all change both the buy price and the amount of material removed. A part with a large central pocket is often cheaper from tube than from solid bar, because the hole already exists.

One practical rule: specify a material by its function, not by habit. If the part only needs corrosion resistance and light load, 6061 with hardcoat anodizing may do the job of 316 stainless at a much lower machining cost. If it needs wear resistance at temperature, the cheaper alloy fails and you pay twice.

• 1
  Easy to machine6061-T6, 7075, 303 stainless, C36000 brass, POM.
• 2
  Moderate304 and 316 stainless, 4140 steel, 17-4PH, AZ31B magnesium.
• 3
  Slow and tool-hungryTi-6Al-4V, Inconel, hardened tool steel above 45 HRC.

A simple block with four holes and a chamfer is a short cycle. The same block with a 0.8 mm wall, a deep 6:1 bore and a blended fillet is a long cycle, because the tool has to be small, the step-over has to be fine, and the operator has to slow down to avoid chatter. Deep pockets and thin walls are the two features that most often turn a cheap part into an expensive one.

Tolerance works the same way. Marking the whole drawing at ±0.005 mm forces the shop to treat every dimension as critical, which means more in-process checks, more temperature care and possibly a slower finishing pass. If only the bearing bore and the mounting face need ±0.005 mm, say so and leave the rest at general tolerance. The price usually drops without any loss of function.

Surface finish callouts behave like tolerance. Ra 0.2–0.8 μm on an optical face is reasonable. The same callout on a bracket that sits inside a housing adds polishing time for no benefit. Specify Ra per face and note which faces are cosmetic.

Undercuts, sharp internal corners and threads that stop against a shoulder all limit tool access. A corner radius of at least one third of the pocket depth usually lets a larger cutter reach the bottom, which shortens the cycle noticeably.

The hourly rate of a 5-axis machining center is higher than a 3-axis mill. That does not mean 5-axis parts are always more expensive. The comparison that matters is total time in the shop, including setups.

A part with features on five faces, or with angled holes and compound surfaces, needs multiple fixtures on a 3-axis machine. Each fixture costs design time, build time and a first-article check. With simultaneous 5-axis machining, the part often stays in one vise for the whole cycle. On a complex housing, that alone can remove several hours of setup and handling.

4-axis machining sits in the middle. It is a good fit for cylindrical parts with cross holes or flats, where the rotary table indexes the part between operations. If the geometry is mostly rotational, a mill-turn center may be even better, because turning and milling happen in one program with one datum.

When 5-axis does not pay off: flat plates, simple shafts, prismatic parts reachable from one or two sides, and parts where the tolerance is dominated by a single bored hole. On those, a 3-axis machine with a good fixture is faster and cheaper.

Setup cost is fixed per batch. Programming, fixturing and first-article inspection happen once whether you order one part or one thousand. That is why the first part is always the most expensive one you will ever buy from a given design.

As quantity rises, the setup is spread across more parts, and the shop can also optimize the process: dedicated fixtures, custom soft jaws, tool paths tuned for tool life rather than for finishing the single part quickly. In many cases the cycle time per part at 500 pieces is lower than at 5 pieces, because the programmer no longer has to be conservative.

The curve flattens at some point. Once setup is negligible and the process is stable, the price per part approaches material plus cycle time plus inspection. Asking for a price break beyond that point usually means changing the process: casting, die casting, or a different stock form.

This is also where prototyping and production should be planned together. If the prototype is machined from solid but the production part will be die cast, the two parts will not behave the same under load. Decide the production process before the design is frozen.

Finishing is usually quoted per part or per batch, and the driver is surface area plus handling. Bead blasting and tumbling are inexpensive and hide tool marks. Anodizing adds a color and a corrosion layer but changes dimensions slightly, so thread and bore allowances should be checked before the finish is applied. Hardcoat anodizing builds more thickness than clear anodizing and can close a tight tolerance.

Plating options such as electroless nickel, zinc, silver and gold are priced by area and by rack space. Small parts with many separate pieces can cost more to rack than to machine. Laser marking is cheap but has a minimum character height of 1.5 mm, so fine text may not survive.

Inspection is the line item most often left vague. A standard quote may include a dimensional report on a few features. Full CMM inspection of every part, with a report per serial number, is a different scope. For medical and aerospace work this is normal; for an internal bracket it is usually overkill.

Ask for the inspection plan in writing. Which features are measured, with what instrument, and how often. That answer tells you more about the supplier than the price does.