Machining 2: the second-pass decisions that decide part cost

• 1
  Why the second pass behaves differently
• 2
  Setup consolidation and the error stack
• 3
  Thin walls, deep pockets and tool reach
• 4
  Where tolerance stops paying for itself
• 5
  Material choice and what it does to the process
• 6
  How a second-pass design gets verified
• 7
  Which setup suits which geometry

The first pass proves a geometry can be cut. The second pass proves it can be cut repeatedly, at a cost that survives volume. Those are different problems, and the second one is where most schedules slip.

Machining 2 work usually means the part already exists as a prototype. The alloy is chosen, the finish is agreed, and the discussion moves to setup count, fixture design, and where the datums sit. A design that needed four setups in prototyping may need two in production, or it may need six once inspection gauges are added.

The physics does not change between passes. The tool still shears material, the spindle still deflects under load, and heat still moves through the workpiece. What changes is how much of that variation you can absorb before the part misses print.

On a prototype, an operator can adjust offsets mid-run. On a 10,000-part order, the process has to hold without that attention. That is the real subject of this page.

• 1
  Setup count drives costEach additional fixturing adds load and unload time plus a new source of position error.
• 2
  Datums movePrototype datums are often chosen for inspection convenience, not for machining access.
• 3
  Stiffness matters more at volumeA wall that survived one part may chatter on the five hundredth.

Every time a part is unclamped and re-clamped, a new position error enters the stack. If a feature is cut in setup one and a related feature in setup three, the tolerance between them is the sum of the fixture repeatability, the datum transfer, and the machine's positioning error. On a machine that holds ±0.005 mm in a single setup, a three-setup part can easily drift to ±0.02 mm or worse between features.

The usual fix is to move work into a 5-axis setup. With 16 simultaneous 5-axis machining centers on our floor, a part that needs five faces can often be cut in two setups instead of five. Fewer setups means fewer datum transfers, and it also means less queue time between operations.

Consolidation is not free. A 5-axis fixture often needs more clearance, and the tool has to reach the feature from an angle that may be less rigid than a straight Z cut. For deep pockets with a small corner radius, a dedicated 3-axis setup with a long reach tool can still be the better choice.

The judgment call: consolidate when the tolerance stack or the schedule is the problem; keep separate setups when the geometry needs maximum rigidity and the tolerance is loose enough to absorb the transfer error.

• 1
  Count the transfersList every datum transfer and ask what each one adds to the total error.
• 2
  Check fixture clearanceA 5-axis fixture must clear the tool at every angle, not just the first one.
• 3
  Do not consolidate blindlyRigid 3-axis cuts still win on deep, tight-corner pockets.

A wall's behavior depends on its height-to-thickness ratio. Below roughly 4:1, a wall in aluminium 6061 usually cuts clean with normal parameters. Between 4:1 and 10:1, deflection starts to show and the wall may spring back after the cut, leaving it thicker at the top than the middle. Above 10:1, chatter becomes the default outcome unless the tool path is changed.

The practical workarounds are known. Take lighter radial cuts, use a tool with a smaller diameter and a shorter flute length, support the wall with a temporary web, or leave a finishing allowance and take it in two passes. None of these are free. Each adds cycle time.

Deep pockets have a related problem: tool reach. A cutter that is long enough to reach the floor is also flexible enough to deflect. The rule of thumb is to keep the tool's length-to-diameter ratio under 4:1 for roughing and under 6:1 for finishing, and to reduce feed per tooth as the ratio grows.

For pockets deeper than about 5× the tool diameter, consider whether the feature has to be milled at all. On some parts, an EDM or a drilled corner relief removes the requirement and cuts the cycle time.

• 1
  Wall ratio guideUnder 4:1 cuts clean; 4:1 to 10:1 needs light passes; above 10:1 needs support.
• 2
  Tool L:D guideUnder 4:1 for roughing, under 6:1 for finishing, then reduce feed per tooth.
• 3
  Corner reliefA drilled relief lets a larger cutter reach the pocket floor.

Tolerance is not a single number. It is a cost curve. A dimension held at ±0.1 mm is routine on a 3-axis mill. Tighten it to ±0.02 mm and the process needs temperature control, a warm-up cycle, and more frequent in-process checks. Tighten it to ±0.005 mm and the part may need to be cut, measured on a CMM, and adjusted.

The mistake we see most often is uniform tolerance. A drawing where every dimension is ±0.01 mm forces the shop to treat a mounting boss and a cosmetic edge with the same care. Identify the two or three dimensions that actually control function, and loosen the rest.

Our floor holds ±0.005 mm (±0.0002 in) where the design requires it. That number is a capability, not a default. Applying it broadly raises cost without improving the assembly.

Surface finish follows a similar curve. As-machined at Ra 1.6–3.2 μm covers most brackets and housings. Ra 0.8–1.6 μm is common for sealing faces and sliding surfaces. Ra 0.2–0.8 μm usually requires a separate finishing operation and should be reserved for bearing bores or optical seats.

• 1
  Tolerance selectivelyTighten only the dimensions that control fit or function.
• 2
  Finish follows functionRa 1.6–3.2 μm for general parts, finer only where the surface does work.
• 3
  Inspection adds costEvery extra check point adds handling time and a chance of damage.

Aluminium 6061-T6 is the default for most machined parts. It cuts fast, holds a good finish, and takes anodizing well. The 7075 grade is stronger but more prone to stress movement after heavy material removal, so it usually needs a roughing pass, a stress-relief pause, and a finishing pass.

Stainless 303 machines freely because of its sulfur content, which makes it the first choice for turned parts. The 304 and 316 grades are tougher on tooling and work-harden if the cutter dwells. Keep the feed per tooth up and never let the tool rub.

Titanium TC4 (Ti-6Al-4V) and Inconel sit at the other end. They cut hot, wear tools quickly, and need lower surface speeds, more coolant, and rigid setups. A part in Inconel that would cost one unit in aluminium may cost four or more, mostly in tool changes and cycle time.

Plastics behave differently. POM and PEEK cut cleanly but move with temperature, so dimensions measured right after the cut may not match dimensions measured the next morning. For tight plastic parts, let the part stabilize before final inspection.

• 1
  6061-T6 is the baselineFast, stable, anodizes well. Start here unless strength says otherwise.
• 2
  7075 needs stress reliefRough, pause, finish, or the part may bow after the last cut.
• 3
  Never rub stainlessWork hardening turns a light pass into a scrapped part.

Verification starts at the drawing. We run a free DFM analysis with every quote, usually within 12 hours, and the review flags features that will be hard to hold: unsupported walls, deep slots with sharp internal corners, threads that run into a shoulder, and tolerance callouts that do not match the function.

The first article is the real test. It is cut on the production fixture with production parameters, then inspected across every dimension that matters. If the first article passes, production can start within 24 hours. If it drifts, we adjust the process rather than the inspection plan.

Production parts ship in 3–5 days for most work, with 100% inspection before shipment covering raw material check, in-process monitoring, and final inspection. Reports are available on request.

The point of all this checking is not paperwork. It is to catch a design decision that only shows up once the part exists, while the fix is still cheap.

• 1
  Free DFM per quoteFlagged features come back with the price, usually within 12 hours.
• 2
  First article on production toolingTesting on prototype fixtures does not prove the production process.
• 3
  Fix the process, not the reportAdjusting inspection to pass a drifting process hides the problem.