Basic Knowledge of CNC Analysis

CNC analysis starts with the CAD file, not the machine. Someone opens the model and checks whether every surface can be reached by a tool that physically exists. A pocket with a 3 mm corner radius needs a 6 mm cutter to clear it, and that cutter has to reach the bottom without the holder rubbing the wall. If the wall is 40 mm tall, the holder hits first. That is a geometry problem, not a programming problem.

Next comes the drawing. Dimensions, datums and callouts get matched against the model. When a dimension is missing, the machinist guesses, and a guess on a datum is how a good part ends up rejected at inspection. We flag missing datums, ambiguous tolerances and any feature that is dimensioned to a surface that will be removed later.

The last check at this stage is the material. Aluminum 6061 cuts freely and holds a sharp edge. Stainless 316 work-hardens if the feed is too light, so a finishing pass that works on aluminum can ruin a 316 bore. Inconel and Ti-6Al-4V move heat into the tool instead of the chip, which changes speeds, feeds and sometimes the whole setup plan. Analysis without material data is only half done.

The output of this step is short: a list of features that need a design change, a note on which tolerances drive the setup, and a first guess at how many operations the part needs.

• 1
  Deep pocketsCheck depth-to-diameter ratio before quoting; over 4:1 usually needs a smaller cutter and longer cycle.
• 2
  Thin wallsBelow 0.8 mm on aluminum, deflection shows up as taper unless supports or light passes are used.
• 3
  Sharp internal cornersA cutter leaves its own radius; state the corner radius you can accept.

CAM software turns the model into toolpaths, and the post-processor turns those paths into G-code the controller understands. The controller reads each block, moves the axes, and monitors spindle load, feed override and tool life. On a 3-axis machine the tool axis stays vertical. On a 5-axis center the table or the head tilts, so a single setup can reach five faces of a part without re-clamping.

The reason this matters to a designer is setup count. Every time a part is unclamped and re-fixtured, the new zero point introduces error. A part that needs five setups on a 3-axis mill carries five chances to drift. The same part on a 5-axis center may need two. That is why a face with a tight true-position callout is often cheaper on a 5-axis machine even though the hourly rate is higher.

Cutting tool choice follows the same logic. A face mill removes material fast but leaves a coarser floor. A bull-nose cutter splits the difference. A ball-nose tool is the only way to follow a curved surface, and it must step over in small increments to keep the scallop height low. Each choice trades cycle time against surface finish.

Simulation runs before metal is cut. It catches tool-holder collisions, rapid moves through stock, and toolpaths that violate the fixture. A collision caught on screen costs nothing. The same collision on a 30,000 rpm spindle costs a holder, a tool and a day.

A general tolerance block of ±0.1 mm is easy. A single ±0.005 mm callout on one bore changes the plan for the whole part. That bore will probably be finished on a separate operation, checked with a bore gauge or CMM, and possibly re-cut if it drifts. Tight tolerances are fine. Tight tolerances scattered across a drawing without a reason are expensive.

The usual trap is tolerance stacking. If three features are each held to ±0.05 mm and their positions depend on one another, the assembly may still fail. Ask which dimension the function depends on, then tighten that one and loosen the rest. A drawing where one datum chain carries the precision and everything else is loose machines faster and inspects faster.

Geometric callouts deserve the same treatment. Flatness, perpendicularity and true position are all measurable, but each one needs a datum to measure from. A true-position callout with no datum reference cannot be inspected, so it will be argued about at the receiving dock. Put the datum on the drawing.

On our side, tolerance capability sits at ±0.005 mm (±0.0002 in) on the machines that can hold it. We say which features those are rather than quoting the number for the whole part.

Material decides feeds, speeds, tool coating and sometimes the machine. Aluminum 6061, 2024 and 7075 all cut well, but 7075 is stronger and more prone to stress movement after heavy stock removal. Stainless 303 is free-machining; 304 and 316 are not, and 316L galls against a dull tool. Titanium TC4 and Inconel need low surface speed, high pressure coolant and a rigid setup, so they run slower and cost more per part.

Plastic parts follow different rules. POM and PA want sharp tools and air blast rather than flood coolant. PEEK tolerates heat but is abrasive on tooling. ABS and PMMA are soft enough that clamping pressure marks the surface, so soft jaws or vacuum fixturing are used instead of a hard vise.

Setup planning comes out of all this. A part with two flat faces and a bore might be a two-op job on a 3-axis mill. A part with features on five sides and a Ø400 mm bolt circle on the bottom belongs on a 5-axis center or a mill-turn machine. Mill-turn centers are useful when the part is mostly round with a few milled flats, because turning and milling happen without a second fixture.

Our floor covers 127 CNC machines, including 16 simultaneous 5-axis centers, 12 four-axis mills, 27 three-axis machines and 16 mill-turn centers. Maximum processing size is 4,000 mm. That range matters during analysis: the setup we choose is the one that fits the part, not the one that is free.

CNC analysis should end with a process recommendation, and sometimes that recommendation is not CNC. A thin sheet-metal bracket with no machined features is faster and cheaper stamped or laser cut and bent. A hollow shell with uniform 2 mm walls is a better fit for die casting or vacuum casting once volumes pass a few hundred pieces.

CNC wins when geometry is complex, quantities are low, or the material is hard to cast. A prototype bracket, a fixture plate, a one-off manifold or a housing with five bored faces all suit machining. It also wins when the part will be revised. Changing a program takes minutes; changing a mold does not.

There is a volume line worth knowing. Below roughly 500 pieces, machining usually beats tooling cost. Above a few thousand, a casting or molding process spreads its tooling across enough parts to win. Between those points the answer depends on tolerance and surface finish, and that is a calculation rather than a rule.

If a design has features that only exist because of an assembly problem, fix the assembly first. Machining a hard-to-reach pocket to hold a screw that could be relocated is cost without benefit.

• 1
  Prototypes and one-offsMachining avoids tooling cost and allows same-week changes.
• 2
  Hard materialsTitanium, Inconel and hardened tool steel are machined, not cast.
• 3
  High volume, simple shapeCasting, molding or stamping take over as quantity grows.