CNC CAD drawing essentials: what CAM needs before the first cut

• 1
  Why a clean solid model is the first of the CNC CAD drawing essentials
• 2
  GD&T and datum strategy that survive machining
• 3
  Material callouts change the toolpath, not just the price
• 4
  Surface finish symbols and where they apply
• 5
  Where a drawing fights the five-axis process
• 6
  How material choice sets the machining window
• 7
  What belongs in the model versus the drawing

CAM software does not read your intent. It reads surfaces, and it connects them into a toolpath. If the solid is not watertight, the software has to guess where the material ends. That guess becomes a gouge, a sliver of stock left behind, or a toolpath that fails to generate at all.

The common defect is a non-manifold body: two faces sharing one edge, a gap of 0.02 mm between two surfaces that should be joined, or a self-intersecting fillet where three radii meet. None of these show up in a shaded view. They show up when the CAM kernel tries to offset the surface for cutter compensation.

Run a repair pass before export. In SolidWorks use Check Entity; in Fusion 360 use Validate. Look for minimum edge length, knife-edge faces and zero-thickness walls. A wall thinner than 0.5 mm in aluminium will chatter or deflect, even if the geometry is mathematically valid.

Export the format your shop actually uses. STEP AP242 carries PMI data and is the safest general choice. Native files (SLDPRT, IPT) keep the feature tree, which helps when we need to adjust a fillet rather than rebuild it. STL is a mesh, not a drawing, and it loses every tolerance you specified.

• 1
  WatertightOne closed body. No gaps, no overlapping faces, no stray surfaces.
• 2
  Single scaleModel at 1:1 in millimetres or inches. Never scale a STEP at import.
• 3
  Real datumsPlace the origin where the part will be clamped, not at a random corner.

A drawing that dimensions every feature from a different corner forces the machinist to stack tolerances manually. Use GD&T properly and the stack is handled by the datum reference frame. Pick three datums: a primary plane that sits flat on the vise or fixture, a secondary that locates one edge, and a tertiary for rotation.

The primary datum should be a surface the part actually rests on. If you nominate a small boss as datum A, the setup becomes unstable and every downstream tolerance inherits that instability. On a five-axis part, the primary datum is usually the face that gets machined first, because that face is then flat for the second operation.

Position tolerance with MMC (maximum material condition) is generous to the shop. It allows bonus tolerance as a hole grows, which often turns an unmakeable callout into a routine one. A hole at Ø6 H7 with a true position of 0.05 mm at MMC is a different job from the same hole at RFS.

Keep the number of tight callouts small. If a bracket has 40 dimensions and 12 of them are ±0.01 mm, the part will be inspected slowly and the cost reflects that. Ask which three features actually set the function. Tolerance those tightly, and open the rest to general tolerance.

• 1
  Datum A on a real resting faceNot a cosmetic boss or a freeform surface.
• 2
  MMC where possibleBonus tolerance reduces scrap on hole patterns.
• 3
  General tolerance blockState it. It stops every unfigured edge from becoming a debate.

Aluminium 6061-T6 machines at 300–600 m/min surface speed with carbide. Titanium Ti-6Al-4V runs at 40–60 m/min and work-hardens if the cutter dwells. The same geometry, drawn once, becomes two different processes. That is why the material callout is not a purchasing field; it is a machining instruction.

Temper matters as much as alloy. 6061-T6 is stable and predictable. 6061-O is gummy and builds a built-up edge on the cutter. 17-4PH in the H900 condition cuts cleanly; in the annealed condition it smears. If you specify the alloy without the temper, the shop has to guess and the surface finish will drift.

Stock size and grain direction belong on the drawing too. A part 300 mm long cut from 20 mm plate has different residual stress behaviour than the same part cut from extruded bar. Thin plate can bow after the first face is removed. We plan roughing passes and stress-relief stops around that, but only if we know the stock form.

For plastics, the callout needs more detail, not less. POM and PEEK move with temperature. A tolerance of ±0.02 mm on a 200 mm PEEK part may be unmeasurable at 20 °C and wrong at 40 °C. Note the inspection temperature if the fit is critical.

• 1
  Alloy plus temper6061-T6, not just 6061. 17-4PH H900, not just 17-4PH.
• 2
  Stock formPlate, bar, extrusion or casting changes the stress path.
• 3
  Heat treat sequenceSay whether hardening happens before or after machining.

Ra 1.6 μm is the default machined finish on most parts. It comes off a sharp carbide cutter at moderate feed and needs no extra operation. Ra 0.8–1.6 μm is achievable on the same setup with a lighter finish pass. Below Ra 0.8 μm you are into polishing, lapping or a fine step-over on a dedicated finishing tool.

Put the symbol only on the faces that need it. A drawing with a global note of Ra 0.4 μm triples the finishing time and often cannot be measured on a curved surface anyway. Mark the sealing face, the bearing bore and the optical seat. Leave the rest as machined.

Anodizing and plating add thickness. Type II clear anodize builds about 5–15 μm per surface. A Ø10 H7 bore that is masked will stay at size; an unmasked bore will close by roughly twice the coating thickness. Say which features are masked, or the coating will eat your clearance.

Bead blasting hides tool marks but rounds edges. A 0.2 mm chamfer becomes a 0.4 mm radius after a heavy blast. If the drawing calls a sharp edge for safety or function, note it as a masked or protected edge.

• 1
  Ra 0.8–1.6 μmStandard finish pass. No secondary operation.
• 2
  Ra 0.2–0.8 μmFiner step-over or polishing. Budget extra time.
• 3
  Coating buildNote masked features on anodized and plated parts.

Deep pockets with a small corner radius are the classic problem. A 40 mm deep pocket with a 3 mm internal radius needs a 6 mm cutter reaching 13 times its diameter. That tool will deflect. Either open the corner to 6 mm radius or accept a separate EDM or sinker operation.

Undercuts and features on five sides are fine on a simultaneous five-axis center, but they need clearance for the holder, not just the cutter. A feature can be geometrically reachable by the tool tip and still be blocked by the collet nut. When we review a model, we check the holder envelope, not only the tool.

Sharp internal corners in a pocket floor will always carry a small radius from the cutter. If the drawing calls a true 90° internal corner, the note should say whether a corner relief is allowed. Most designers accept a 0.5 mm relief once they see the alternative cost.

Text and logos engraved below 1.5 mm character height tend to fill with chips and read poorly after anodizing. Laser marking holds detail better than milling at that scale, and it does not add a tool change.

• 1
  Pocket depth to diameterKeep under 4:1 for a rigid carbide cutter.
• 2
  Holder clearanceThe nut, not the cutter, is often the limit.
• 3
  Corner reliefAllow a small radius instead of a theoretical sharp corner.