CNC Processing Solid Work: From Model to Machine

• 1
  What CNC processing solid work actually means
• 2
  Which file format carries which information
• 3
  How model features turn into toolpaths
• 4
  Where tolerance and finish come from
• 5
  What we check in a DFM review
• 6
  Model detail versus machining outcome

A solid model is a closed 3D body with real volume. That is the difference from a wireframe or a surface model. Because the body is closed, a CAM system can ask a simple question: where is the material? That single property is what makes solid work usable for machining.

SolidWorks is one common way to build that body. The machine never reads the SolidWorks file. The model leaves the CAD environment as a neutral format, a CAM system rebuilds it, and toolpaths are posted as G-code. Every step in that chain can lose information if the model is loose or the export settings are wrong.

So CNC processing solid work is not a software feature. It is a translation job. The goal is to hand the shop geometry it can trust: closed bodies, clear datums, and callouts that match the drawing. When that happens, programming is fast and the first article usually passes.

When it does not, the shop spends hours rebuilding surfaces that should have been simple. Those hours show up in the quote. Most of the file problems we see are avoidable in under ten minutes of cleanup.

STEP is the default handoff. It carries exact B-rep geometry, so arcs, cones, and fillets stay true. For most turned and milled parts, an AP214 or AP242 STEP file is all we need. It does not carry your feature tree, and that is usually fine.

IGES is older and surface-based. It can break a closed body into separate patches, and holes sometimes arrive as trimmed surfaces instead of cylinders. We still accept it, but expect a repair pass. PARASOLID is similar in quality to STEP and often arrives from other CAD systems.

STL is a mesh. It has no true arcs, only triangles. A 0.05 mm chord tolerance on a 10 mm bore can leave visible flats. Use STL for visual reference or additive work, not for tight CNC tolerances. Native SolidWorks files are welcome when you want us to check the feature tree and sketch relations.

One rule covers most cases: send STEP for the geometry, and send a PDF drawing for the intent. Threads, fits, and datum callouts belong on the drawing, because no neutral format carries them reliably.

• 1
  STEP AP214 / AP242Best all-round choice for milled and turned parts.
• 2
  IGESAcceptable, but may need surface repair before programming.
• 3
  STLMesh only. Keep chord tolerance 0.02 mm or finer if used.
• 4
  PDF drawingCarries threads, fits, datums, and finish callouts.

A CAM programmer picks a stock body, sets a coordinate system, and selects features to cut. A pocket becomes a roughing pass plus a finishing pass. A hole becomes either a drill cycle or a helical bore, depending on diameter and tolerance. The model decides which of those is possible.

Feature size sets the tool. A 3 mm internal corner needs a cutter no larger than 6 mm, and that small cutter must reach the full depth. If the pocket is 40 mm deep, tool deflection becomes the limiting factor, not the machine. Deep narrow pockets are where quotes climb fastest.

Tool access is the other hard limit. A T-slot under an overhang cannot be cut from above. A hole on a face that no spindle can reach needs a different setup or a 5-axis move. On our 16 simultaneous 5-axis centers, a Ø400 mm rotary table lets us tilt the part instead of adding fixtures.

Sharp internal corners are a third limit. A cutter always leaves its own radius. If the model shows a true 90° internal corner, the drawing must say whether that corner is functional or just drawn that way. Undercuts and zero-radius corners are the two features most likely to force a design change.

Tolerance is not one number for the whole part. It is a stack of decisions: machine capability, setup count, tool wear, and thermal drift. Our general machining tolerance is ±0.005 mm on critical features when the geometry and material allow it. Not every dimension needs that.

A useful habit is to split dimensions into three groups. Critical fits get a tight callout. Functional dimensions get a normal one. Cosmetic and clearance dimensions stay loose. This keeps cost down, because tight tolerance drives extra setups, in-process checks, and slower feeds.

Surface finish follows the same logic. As-machined faces sit around Ra 1.6–3.2 μm. A finer Ra 0.8–1.6 μm is common for sealing faces and bearing bores. Ra 0.2–0.8 μm needs slower finishing passes and often a secondary operation. Specify finish only on the faces that touch something.

Material matters here too. Aluminum 6061 and 7075 cut cleanly and hold tight tolerances well. Stainless 316 and 17-4PH work-harden, so light finishing passes and rigid setups matter more. Titanium TC4 (Ti-6Al-4V) and Inconel move under heat, so we plan roughing, cooling, and a separate finishing pass.

Every quote includes a free DFM review, and we return it within 12 hours. The review is not a sales step. It is where we catch the details that would otherwise become a mid-run problem. Production can start within 24 hours once the model and drawing are settled.

We start with wall thickness and corner radii, because those set the tool list. Then we check hole depth-to-diameter ratios. Beyond about 4:1 on a drill, chip evacuation and drill wander become real risks, and we may switch to peck drilling or helical milling.

Next come datums and fixturing. A part with no flat face to clamp on needs soft jaws or a custom fixture, and that is a cost item. We also look at thin floors and tall ribs, since those vibrate and need lighter passes. Five-axis access is checked on any feature that faces away from the main spindle.

The last pass is finish and marking. Anodizing, electroless nickel, and powder coating all add or remove a small amount of material, so masking and pre-finish dimensions matter. Laser marking needs a minimum character height of 1.5 mm to stay readable. If a serial number is required, tell us at quote time, not after.