Medium Parts CNC Machining Guide

• 1
  What counts as a medium part in medium parts CNC machining
• 2
  Why five-axis helps medium parts CNC machining
• 3
  Wall thickness, depth and feature size limits
• 4
  Tolerance and surface finish on medium-sized parts
• 5
  Material choices that fit the 10–300 mm band
• 6
  Choosing a setup for medium parts CNC machining

There is no official cutoff. In our shop, a medium part is anything that fits inside a 600 × 600 × 600 mm work envelope but is too big to be bar-fed on a lathe. That covers a motor housing at Ø180 mm, a robot wrist bracket at 250 mm, a pump body, a manifold block. Below roughly 10 mm the part is usually turned or stamped. Above 300 mm you are into large-frame work where the machine travels, not the part geometry, decide the process.

Size is only half the definition. The other half is feature count. A 200 mm plate with eight holes is a simple job on a 3-axis mill. The same 200 mm plate with pockets on five faces, a 12° draft wall and a seal groove on the side is a different problem. Medium parts CNC machining gets expensive when face count and tolerance stack up at the same time, not when the part is merely big.

The 10 mm to 300 mm band matters because it is where most product hardware lives. Automotive brackets, EV busbar housings, medical instrument bodies, robot joints, valve blocks. These parts carry real loads, seal fluids or hold bearing bores, so the tolerances are tight but the volume is rarely high enough to justify a dedicated fixture line.

One practical check: if the part needs four or more machined faces, or if two bores must stay coaxial over 150 mm, treat it as a five-axis candidate from the start. Re-quoting a part after a failed 3-axis run costs more than the setup difference.

• 1
  10–300 mmTypical span for medium parts; below it, turning and stamping take over.
• 2
  Feature countFive machined faces is the usual tipping point toward 5-axis.
• 3
  Load-carrying partsBearing bores and seal grooves drive the tolerance call.
• 4
  Low volumeFrom one prototype to 10,000+ part runs, fixtures rarely pay off.

A 3-axis mill moves the tool in X, Y and Z. The part stays put. That works until a feature faces sideways. Then you either refixture the part, or you buy a longer tool and hope it reaches. Refixturing a 200 mm part means releasing clamps, repositioning, re-indicating, and accepting the stack-up of two setups. On a bore-to-bore tolerance of ±0.02 mm, two setups can eat the whole budget.

Five-axis adds two rotary axes, usually A and B, so the tool can reach the part at an angle. The gain is not speed. The gain is that the part is cut in one setup, which keeps bore alignment and face squareness inside one datum. Our 5-axis centers run on a Ø400 mm rotary table and cover travels of 750 × 1,150 × 550 mm and 600 × 600 × 600 mm, which fits most medium work without a tombstone.

The second gain is tool access. A deep pocket with a 15 mm corner radius can be cut with a short, stiff tool held at an angle instead of a long slender tool held vertically. Short tools chatter less. Less chatter means you can hold Ra 0.8–1.6 μm without a separate finishing pass, and tool life stops being the bottleneck on hardened 17-4PH or 4140.

The trade is not free. Five-axis programming takes longer, the setup is less forgiving, and the machine hour rate is higher. For a prismatic part with three machined faces and a ±0.05 mm tolerance, a 3-axis quote will be cheaper and just as good. The rule we use: count the faces, count the tight tolerances, and if two or more tight tolerances cross between faces, go five-axis.

• 1
  One setupKeeps bore alignment and squareness inside a single datum.
• 2
  Short toolsAngled access replaces long slender tools that chatter.
• 3
  Higher rateFive-axis hours cost more; spend them where faces cross.

Medium parts often have thin walls because the housing has to be light. Aluminum 6061 walls down to 0.8 mm are machinable, but they deflect under cutting force. In practice we keep structural walls at 1.5 mm minimum and go thinner only on short, supported sections. A 0.8 mm wall on a 120 mm tall pocket will sing, and the finished part will show a taper you did not ask for.

Stainless behaves differently. 304 and 316 work-harden, so the first pass has to bite under the hardened layer. Walls at 2 mm are comfortable; below 1.2 mm the part tends to move between roughing and finishing. If the drawing calls for a 1 mm wall in 316L, expect to rough, stress-relieve with a pause, then finish, and budget the extra time.

Pocket depth is the other limit. A rule of thumb is 4:1 depth to tool diameter for a rigid carbide end mill, 6:1 with a reduced feed. So a 40 mm deep pocket is fine with a 10 mm tool. A 120 mm deep bore needs a 20 mm tool, or a different process. Deep bores also need coolant through the tool, otherwise chips pack at the bottom and you break the cutter.

Small features have their own floor. A slot narrower than 1 mm needs a micro tool that breaks easily, and a thread below M2 is better cut with a thread mill than a tap. For laser marking, minimum character height is 1.5 mm. If your part number has to be readable after anodizing, size the text accordingly.

• 1
  Aluminum walls0.8 mm possible on short sections; keep 1.5 mm structural.
• 2
  Stainless walls2 mm comfortable in 304/316; below 1.2 mm expect movement.
• 3
  Pocket depth4:1 depth-to-diameter for rigid carbide, 6:1 with reduced feed.
• 4
  MarkingLaser marking minimum character height 1.5 mm.

A ±0.005 mm tolerance is achievable on medium parts, but not everywhere on the part. It applies to the features that matter: bearing bores, dowel holes, mating faces. If the whole drawing carries ±0.005 mm, the quote goes up because every operation has to be stabilized, including temperature. Aluminum grows about 23 μm per meter per degree Celsius, so a 200 mm part that warms 5 °C during machining moves more than 0.02 mm.

The workable approach is to tolerance the function. Hold ±0.005 mm on the bore, ±0.05 mm on the bolt pattern, and general ±0.1 mm elsewhere. That is not a compromise on quality. It is how a shop spends inspection time where it changes fit. We inspect 100% before shipment and can supply reports on request.

Surface finish follows the same logic. As-machined faces land at Ra 1.6–3.2 μm. A sealing face needs Ra 0.8–1.6 μm, which usually means a separate finishing pass with a sharper insert and a lighter depth of cut. Optical or vacuum sealing surfaces go to Ra 0.2–0.8 μm, and that is where polishing or lapping enters the process chain.

Finish also interacts with coating. Anodizing adds a few micrometers of oxide, and hardcoat adds more. If a bore has to stay at Ø20 H7 after hardcoat, tell the shop before machining, not after, because the machinist has to cut undersize and let the coating bring it back.

• 1
  Tolerance the function±0.005 mm on bores, looser on bolt patterns, ±0.1 mm general.
• 2
  Thermal driftAluminum moves about 23 μm/m per °C; stabilize long cuts.
• 3
  Sealing facesRa 0.8–1.6 μm needs a separate, lighter finishing pass.
• 4
  Coating growthTell the machinist before cutting if a bore must stay H7 after hardcoat.

Aluminum is the default for medium parts because it cuts fast and holds tolerance well. 6061-T6 covers most housings and brackets. 7075 gives more strength for a robot arm or a stressed bracket, at the cost of a slower cut and a bigger bill. 2024 machines well but is less corrosion-resistant, so it usually gets anodized. For die-cast housings that then get machined, ADC12 is common.

Stainless is chosen for corrosion or medical contact. 303 cuts easily but is not weldable. 304 and 316L are the workhorses. 17-4PH (SUS630) can be aged to high strength and still machined, which suits valve stems and pump shafts. 440C goes to bearing races and wear plates. Expect stainless to run at roughly half the cutting speed of 6061, which shows up directly in the price.

Steel enters when the part takes real load. 4140 and 4340 are the standard for shafts and housings that get heat-treated. 1018 is for simple fixtures. 4130 is common in aerospace airframe parts. Tool steel is used for dies and wear surfaces. All of these machine fine in the medium band, but pre-hardened stock above 40 HRC needs carbide and reduced depth of cut.

Titanium and nickel alloys are the slow end. TC4 (Ti-6Al-4V) and Inconel both hold strength at temperature and resist corrosion, and both are hard on tooling. Inconel especially wants low surface speed and generous coolant. If a medium part has to be Inconel, the geometry should be as simple as the function allows, because every extra pocket costs more than it would in aluminum.

Plastics round out the list. POM and PA for wear parts, PEEK for high temperature and chemical resistance, PC and PMMA for clear covers. Plastics machine fast but move after cutting, so a 200 mm POM plate may need a stress-relief pause between roughing and finishing.

• 1
  Aluminum6061-T6 default; 7075 for stressed brackets; ADC12 for cast housings.
• 2
  Stainless303 free-cutting, 304/316L corrosion, 17-4PH for aged strength.
• 3
  Steel4140 and 4340 for heat-treated load parts; 4130 in airframe work.
• 4
  TitaniumTC4 and Inconel machine slowly; keep geometry simple.