How to Prepare CAD Files for CNC Machining

• 1
  Key takeaways
• 2
  What prepare CAD files for CNC machining actually means
• 3
  Make the model a closed solid before anything else
• 4
  Units, origin and datum setup
• 5
  Tolerances, threads and surface finish callouts
• 6
  Choose the right export format
• 7
  Design choices that raise cost or block a quote
• 8
  Step by step: prepare CAD files for CNC machining
• 9
  Which CAD file format to send for machining
• 10
  When a feature is ready to machine and when it is not

A machinist reads your model as a set of boundaries. Every face, hole and pocket becomes a cutter path with a real tool diameter and a real depth of cut. So the job of preparing a file is not cosmetic. It is making those boundaries unambiguous, so the quote reflects the part you designed.

Most delays we see are not caused by hard geometry. They come from a model that is a surface quilt instead of a solid, a part drawn at the wrong scale, or a thread note that lives in someone's head. Fixing those three things before upload removes most back-and-forth.

We quote and run parts from one prototype to 10,000+ piece runs, with no minimum order quantity. Material choices run from aluminium 6061 and 7075 to 17-4PH stainless, Ti-6Al-4V and PEEK. None of that matters if the file arrives open-ended.

This page is the sequence we would follow ourselves. Model hygiene first, then units and origin, then tolerances and callouts, then export and handoff.

A CNC program needs a volume to cut away from. If your part is a collection of trimmed surfaces, the CAM system has to guess where the inside is. Sometimes it succeeds, and you get a quote. Sometimes it fails, and the shop asks you to repair the model first.

In SolidWorks, check with Tools > Check. In Fusion 360, run Validate in the Inspect menu. In Siemens NX, use Examine Geometry. You are looking for the same three things: open edges, self-intersecting faces, and zero-thickness walls.

Zero-thickness walls deserve a separate mention. A 0.05 mm rib in a plastic part that will be injection molded is a real feature. The same rib in machined aluminium is a broken end mill. Give any wall that a cutter will pass along at least 0.8 mm of thickness, and prefer 1.5 mm or more.

If you model in a surface-based tool like Rhino or Alias, close the solid before export. Most CAD packages have a stitching or join command that will report the remaining gap width. Anything above 0.01 mm is worth fixing, not leaving for the shop.

• 1
  Watertight bodyOne solid, no stray surfaces or construction planes left visible.
• 2
  No self-intersectionFillets that fold back on themselves are a common hidden error.
• 3
  Minimum wallKeep machined walls at 0.8 mm or thicker for aluminium and steel.

Set your document units to millimeters or inches at the start, and stay consistent. A part modeled in inches but exported from a millimeter template comes out 25.4× small. Shops catch this, but it costs a day of confirmation.

Place the model origin somewhere meaningful. The best choice is a corner or a face that also appears on your drawing as a datum. When the origin sits in the middle of empty space, the programmer has to invent a zero point, and that invented zero is where setup errors creep in.

For prismatic parts, align the model to the axes. Put the primary flat face on the XY plane and the longest straight edge along X. Five-axis work can tolerate an odd orientation, but three-axis work is far quicker to program when the part sits square to the machine.

If the part is a turned component, the axis of revolution should sit on the Z axis or the X axis, whichever your shop expects. Tell them which one in the drawing notes. This single sentence saves a setup discussion.

Model everything at nominal size. Do not shrink a bore by 0.01 mm to bias the fit. If a hole needs to be reamed, say so on the drawing with a tolerance band. The machinist will pick the tool and the compensation to hit it.

General tolerances should be stated once, in the title block. A typical shop default for machined metal is ±0.1 mm on untoleranced dimensions. Critical dimensions then get their own callouts. We hold ±0.005 mm (±0.0002 in) on features that require it, but only when the drawing says which features those are.

Threads should be called out with the standard name, not modeled as a cosmetic helix. Write M6 × 1.0 or 1/4-20 UNC in the drawing. A modeled thread adds file weight and gives the programmer no useful information. A thread table is clearer and cheaper.

Surface finish goes the same way. Ra 1.6–3.2 μm is a normal as-machined finish. Ra 0.8–1.6 μm needs a finishing pass and a finer stepover. Ra 0.2–0.8 μm usually means a secondary operation. Naming the finish per face tells the shop where to spend time and where not to.

• 1
  Nominal modelKeep design intent on the drawing, not in a shifted model.
• 2
  One general toleranceState it in the title block; call out exceptions individually.
• 3
  Named threadsUse M6 × 1.0 or 1/4-20 UNC text instead of modeled helices.
• 4
  Finish per faceRa 1.6–3.2 μm default, tighter values only where needed.

For most jobs, send a STEP file. STEP AP214 carries solid geometry, colours and assembly structure, and every CAM system reads it. It is the safest default because it does not depend on which CAD seat you use.

IGES is older and surface-oriented. It can work, but it loses solid information, so a simple cube may arrive as six separate faces. Use IGES only when the receiving shop asks for it. Native files (SLDPRT, SLDASM, IPT, CATPart, PRT) are useful when you want DFM feedback on features, but version compatibility has to be checked first.

Do not send STL for machining unless nothing else exists. STL is tessellated. A hole that should be a true cylinder becomes a ring of flat triangles. The shop can machine from it, but the dimensions will drift, and nobody can measure against a faceted surface with confidence.

If your part has a complex organic surface, add the native file alongside the STEP. That lets the engineer look at the feature tree and suggest a better toolpath or a split part, rather than guessing at how the surface was built.

Sharp internal corners are the single biggest driver of cost on prismatic parts. Every inside corner is cut by a round tool, so the smallest corner radius sets the tool diameter. A 0.5 mm inside radius at the bottom of a 20 mm deep pocket needs a long, thin cutter that must run slowly.

Deep holes behave the same way. A hole deeper than 8× its diameter needs peck drilling and often a pilot drill, and holes past 20× diameter may need gun drilling or EDM, which changes the process entirely.

Thin floors and unsupported walls vibrate. If a machined wall is 0.5 mm thick and 30 mm tall, the part will chatter no matter how good the setup is. Adding a 2 mm rib or leaving a sacrificial web that gets removed later is often cheaper than fighting the vibration.

Finally, tight tolerances applied everywhere are expensive and pointless. Marking a whole part ±0.01 mm when only two bores mate with a bearing triples inspection time and does not improve the assembly.

• 1
  Corner radiusKeep inside corners at 1.2× the intended tool radius or larger.
• 2
  Hole depthStay under 8× diameter where possible; flag anything deeper.
• 3
  Wall thicknessUse 1.5 mm minimum for machined metal walls, more if tall.