CNC machining restrictions: where the process stops

• 1
  Restrictions that come from tool reach and part stiffness
• 2
  Feature restrictions: holes, threads, text and undercuts
• 3
  Tolerance and surface finish limits on real parts
• 4
  Material restrictions: why titanium and Inconel behave differently
• 5
  How to plan around CNC machining restrictions
• 6
  Common CNC machining restrictions and what to do about them

CNC machining restrictions start with a simple fact: a rotating cutter is a rigid cylinder on a fixed axis. It has to physically reach the surface, and the shank behind it has to clear the part. Every restriction below traces back to that reach problem, or to how much the part moves while the tool pushes on it.

Deep pockets are the classic case. A pocket 8 mm wide and 60 mm deep needs a cutter no larger than 8 mm, and a tool that long is slender. Below roughly 4:1 length-to-diameter the tool is stiff enough to cut at normal feeds. Past 6:1 it starts to chatter, and the operator has to slow the feed, which raises cost and often leaves a worse finish on the floor of the pocket.

Sharp internal corners are the second reach problem. A cutter leaves a radius equal to its own radius, so a square internal corner cannot be milled. You can relieve the corner with an undercut, or accept a corner radius. A 3 mm corner radius needs a 6 mm cutter or smaller, which in turn sets the depth you can reach at that corner.

Thin walls and floors are a stiffness problem, not a reach problem. Aluminium walls thinner than about 0.8 mm and steel walls thinner than about 1.0 mm start to deflect under cutting force. Rough the part with extra stock, then take light finishing passes on both sides to balance the load. If the wall is cosmetic only, say so on the drawing.

• 1
  Depth-to-diameterKeep slender tools under 4:1 when you can; 6:1 is the practical ceiling for good finish.
• 2
  Corner radiiInternal radius must be at least half the smallest cutter you allow.
• 3
  Thin wallsBelow 0.8 mm in aluminium the wall may sing or deflect.
• 4
  Deep ribsLeave a draft or a wider root so the tool does not taper into a knife edge.

Hole depth is one of the most common reasons a design gets flagged. A standard twist drill can go about 4× its diameter before chips stop clearing; a carbide drill with through-coolant reaches 10× or more, but the cost per hole rises and the drill may wander at the entry. A Ø3 mm hole 60 mm deep is a gun-drilling job, not a milling job.

Very small holes have their own floor. Below about Ø0.5 mm the tool is fragile, spindle speed matters more than feed, and a broken drill inside the part is expensive to remove. If the hole is only a vent or a light path, consider drilling it in a separate operation or leaving it to the assembly stage.

Threads follow the same rule. A tapped hole needs clearance at the bottom for the tap's lead-in, so blind tapped holes are usually specified at least 1.5× diameter deeper than the thread itself. Thread milling avoids that lead-in and lets you put a thread close to a shoulder, at a higher hourly cost.

Engraved text and part marking have a hard minimum. Our laser marking needs a character height of at least 1.5 mm to stay legible after anodizing or plating. Raised text on a machined face is better at 2 mm and above, and it should sit on a flat, not on a slope or a fillet.

• 1
  Drill depth4× diameter for standard drills, 10× with through-coolant carbide.
• 2
  Blind tapped holesAdd 1.5× diameter of depth for tap lead-in.
• 3
  Laser markingMinimum character height 1.5 mm.
• 4
  Raised textKeep it 2 mm or taller and on a flat face.

Tolerance is a system capability, not a machine setting. We work to ±0.005 mm on features that are reachable, rigid and measurable. That number does not apply to a thin wall 150 mm from the vise, or to a deep bore where the boring bar flexes. On those features ±0.02 mm is a realistic target, and we will tell you so at the quote stage.

The datum matters more than the tolerance value. If a drawing calls ±0.01 mm between two faces that are machined in two separate setups, the error stack includes fixture repeatability. Put the tight tolerance on features cut in one setup, or accept a looser band across setups. This is the single biggest cause of parts that pass inspection on the machine and fail on the CMM.

Surface finish runs on a similar curve. Ra 1.6–3.2 μm is standard as-machined. Ra 0.8–1.6 μm is normal for a finishing pass with a sharp tool and light feed. Ra 0.2–0.8 μm needs a dedicated finishing operation, a small stepover, and often a polished or lapped tool edge. It also costs time, because the finishing pass cannot remove much material.

Some surfaces cannot be cut at all. A deep, narrow slot with a mirror finish on its floor is a case where the tool simply is not long enough and stiff enough to do both. Grinding, EDM or a secondary polishing step may be the answer, and that changes the process plan and the price.

• 1
  Hold ±0.005 mmOnly on rigid, reachable, single-setup features.
• 2
  Across setupsPlan for ±0.02 mm once the part moves between fixtures.
• 3
  Finishing passRa 0.8–1.6 μm is a normal light finishing cut.
• 4
  Mirror finishesRa 0.2–0.8 μm may need lapping or polishing after milling.

Material choice changes the cutting physics. Aluminium 6061 and 7075 cut fast, clear chips easily and tolerate aggressive feeds. Stainless 304 and 316 work-harden at the surface, so a tool that rubs instead of cuts will harden the next pass and shorten tool life. Tool steel and 17-4PH sit in between.

Titanium TC4 (Ti-6Al-4V) has low thermal conductivity, so heat goes into the cutting edge instead of the chip. Cutting speeds drop, coolant flow matters more, and tool wear is measured in minutes, not hours. Inconel is worse on the same curve. Both can be machined well, but the cycle time and the tooling cost are not the same as aluminium, and a quote that ignores this is a quote that will move later.

Magnesium AZ31B and AZ91D machine easily but bring a fire risk with fine chips. They need dedicated chip handling and a controlled coolant strategy. Beryllium copper cuts well but the dust is a health hazard, so it needs enclosed machining and extraction. Neither is a reason to redesign, but both are reasons to plan the shop floor.

Plastics have their own limits. PEEK and POM hold tolerance well if you control heat; ABS and PP deflect and melt at the tool tip, so you cut them with sharp tools at high speed and low depth. Carbon fibre is abrasive and delaminates if you push the tool too hard, so the feed is conservative and the tool life is short.

• 1
  Stainless 304Work-hardens; keep the tool cutting, never rubbing.
• 2
  Titanium TC4Low conductivity, high edge temperature, short tool life.
• 3
  MagnesiumFine chips are a fire risk; enclosed handling needed.
• 4
  Carbon fibreAbrasive and prone to delamination; light feeds.

The cheapest way to handle a restriction is to design it out before the drawing is released. Ask three questions on every part: can a tool reach the surface, will the part stay still while it is cut, and can the tolerance be measured on the shop floor. If the answer to any of them is no, the part will cost more or need a different process.

Split the part when reach is the problem. A deep internal pocket that needs a 4 mm cutter over 60 mm of depth can often become two plates bolted together, each with an open face that a 12 mm cutter reaches easily. The bolted joint adds fasteners and a sealing face, but the machining time drops and the finish improves.

Relax the tolerance where function allows. A cosmetic pocket depth does not need ±0.01 mm. A bearing bore does. Marking the functional dimensions on the drawing, and leaving the rest at general tolerance, lets the machinist choose the setup that holds the tight features and rough the rest.

Plan the process sequence around the tight features. Rough everything, stress-relieve if the part is thin, then finish the tight faces in one setup. For parts that need Ra 0.2–0.8 μm, add a separate finishing pass after the finishing cut. On 5-axis work we can often finish several faces in one setup, which removes the stack-up error that comes from re-fixturing.

• 1
  Ask three questionsCan a tool reach it, will it stay rigid, can it be measured?
• 2
  Split the partTwo open plates often beat one deep pocket.
• 3
  Mark functional dimsTight tolerances only where function needs them.
• 4
  Finish in one setup5-axis work removes re-fixturing error on tight faces.