How to Make a CAD Drawing for CNC Machine

• 1
  Key takeaways
• 2
  What a CAD drawing for CNC machine work has to contain
• 3
  Set the units, origin, and scale before you draw anything
• 4
  Build the view set and dimension it cleanly
• 5
  Choose tolerance values that match the function
• 6
  Threads, holes, and finish callouts
• 7
  Step by step: from blank model to released drawing
• 8
  Which tolerance and finish to put on which feature

A CAD model and a CAD drawing for CNC machine work are not the same deliverable. The solid tells the CAM programmer where material has to go. The drawing tells the operator and inspector what variation is acceptable. If you send a model only, the shop has to guess at tolerance, and that guess shows up later as a rejected lot.

Three elements carry almost all of the risk: the datum scheme, the tolerance values, and the feature callouts for threads, holes, and surfaces. Get those right and the rest of the sheet is housekeeping. Get them wrong and no amount of clean linework will save the job.

A common pattern we see from first-time buyers is a fully modeled part with no dimensions on the print at all. The geometry is fine, but nothing states whether the 12 mm bore is a locating bore or a clearance hole. That single missing callout can swing the machining method and the price.

So the drawing has to answer three questions for the shop. Where do I hold the part? How close do the critical features need to be? Which features are cosmetic and which are functional? Everything else is detail you can add once those are settled.

• 1
  Model for geometry, drawing for toleranceThe two files serve different readers on the shop floor.
• 2
  Datum, tolerance, calloutsThese three carry nearly all of the manufacturing risk.
• 3
  State function, not just sizeA locating bore and a clearance hole need different limits.

Start in millimeters. Most CAM post-processors default to mm and a drawing that switches units mid-sheet is a reliable way to get a part cut at 25.4 times the intended size. If your customer base is imperial, note the conversion in the title block rather than flipping the drawing units.

Place the model origin at a real manufacturing reference, not at a corner of the bounding box. A natural origin is the center of the primary bore, the mounting face, or a mating corner. When the origin lines up with how the part is held, the CAM programmer spends less time re-datuming.

Keep scale at 1:1 in model space and let the sheet handle the print scale. Detailing at 2:1 to make things fit is fine, but the dimension values must stay true. Overrides that change the number to match a scaled sketch are how drawings become fiction.

Finally, decide the projection convention before the first view goes down. First-angle and third-angle produce mirrored layouts, and a shop reading the wrong convention can machine a left-hand bracket as a right-hand bracket. State the convention in the title block and stay consistent for the whole project.

• 1
  Millimeters firstNote imperial equivalents in the title block, not in the dimensions.
• 2
  Origin on a real referenceBore center, mounting face, or mating corner. Not the bounding box.
• 3
  First angle or third angleDeclare it in the title block and never mix the two.

For a prismatic part, three orthographic views plus one section will usually carry the whole definition. Add a detail view at 5:1 or 10:1 for small features such as a 0.5 mm chamfer or an O-ring groove. An isometric view is useful for orientation but should not carry dimensions unless it is the only view that shows a feature.

Dimension from the datums, not from whichever edge is nearest. A chain of dimensions that starts at a random corner stacks tolerance, so a feature 200 mm away inherits the error of every link in the chain. Baseline dimensioning from a datum keeps each feature independent.

Watch for double dimensioning. If a linear dimension and a geometric control both define the same face, the print is ambiguous. The inspector has to choose, and different inspectors choose differently. Delete the redundant callout and keep the one that matches the function.

Leave the hidden lines on the print if they help the machinist understand internal features, but do not dimension to them. Dimension to visible edges and section cuts. A dimension to a hidden line in an isometric view is one of the fastest ways to generate a DFM query.

• 1
  Three views plus a sectionAdd detail views for small features below 1 mm.
• 2
  Dimension from datumsBaseline beats chain when features sit far apart.
• 3
  No duplicate definitionOne feature, one controlling callout.

A blanket tolerance of ±0.1 mm on a title block covers most non-critical dimensions and keeps the price down. Reserve tighter values for the features that actually need them: bearing bores, seal grooves, dowel holes, and mating pilots. On a typical aluminum bracket, two or three tight features out of forty is normal.

When we machine to ±0.005 mm, we need a reason on the print. That limit is achievable on our 5-axis centers, but it costs inspection time and often a temperature-controlled check. If the feature is a clearance hole, ±0.005 mm is money spent for nothing. If it is a bearing seat, it is the whole point of the part.

Surface finish and tolerance travel together. A bore held to ±0.005 mm usually needs Ra 0.8–1.6 μm or better, because the surface peaks eat into the effective clearance. A cosmetic face at Ra 1.6–3.2 μm is fine as machined and needs no secondary operation.

Use geometric controls where a simple plus-minus cannot express the requirement. Position tolerance for hole patterns, perpendicularity for a mounting face, and concentricity for a rotating part are all cases where GD&T does the job in one frame that would take three linear dimensions otherwise.

• 1
  Blanket ±0.1 mmDefault for non-critical dimensions.
• 2
  Tight where it mattersBearing bores, seal grooves, dowel holes, mating pilots.
• 3
  Finish follows toleranceTight bore usually needs Ra 0.8–1.6 μm or better.

Thread callouts need a class, a depth, and a drill note. An M6 × 1.0 tapped hole at 6H with 15 mm of full thread and a 12 mm pilot depth tells the operator exactly what to do. Writing M6 and stopping there leaves the tap drill, the thread depth, and the class open to interpretation.

For blind holes, state whether the drill point is allowed to break through. A 10 mm deep M5 hole in a 12 mm thick plate sounds safe until the drill tip adds another 4 mm. If the far wall cannot be pierced, say so on the print and give the minimum remaining wall.

Counterbores and countersinks need their own diameter and angle. A 90° countersink for a flat-head screw and a 82° countersink for an imperial flat-head screw are not the same cut, and the hardware will sit proud if the angle is wrong.

Finish callouts belong on the drawing too. Anodizing clear, hardcoat, or electroless nickel changes dimensions by a few micrometres, sometimes more on hardcoat. If a bore is anodized after machining, the print should say whether the pre-plate or post-plate size is the controlled one. Laser marking needs at least 1.5 mm character height, so keep marked text above that.

• 1
  Thread class and depthM6 × 1.0, 6H, 15 mm full thread, 12 mm pilot.
• 2
  Blind hole breakoutState if the drill tip may pierce the far wall.
• 3
  Finish shifts sizeSay whether pre-plate or post-plate dimensions are controlled.