How to Prepare a CAD File for CNC Plastic Machining: STEP, DXF and What Your Machinist Needs
- Shubh Poojara
- 1 day ago
- 9 min read
A machinist can only produce what the file tells them to. When a CAD file is poorly prepared — wrong format, ambiguous tolerances, missing views, conflicting dimensions — the machinist either stops and asks questions, makes assumptions, or produces a part that does not match the designer's intent. All three outcomes cost time and money.
This guide covers exactly what a CNC plastic machining shop needs from you: which file formats to use and why, how to structure your drawing, what tolerance and surface finish callouts actually mean in production, and what the most common submission mistakes are and how to avoid them.
Whether you are submitting a simple bracket or a complex multi-part assembly, getting the file right before submission is the single fastest way to shorten your lead time. For a broader guide on how design decisions affect what the machinist can produce, see our overview of design for manufacturing principles.
Table of Contents
File Formats: STEP, DXF, and When to Use Each
Side-by-side comparison of a STEP file opening in a 3D CAD viewport (dark charcoal engineering environment showing a machined plastic bracket in 3D with datum planes visible) versus a DXF file shown as a flat 2D profile with dimension lines — illustrating when each format is appropriate
STEP Files (.step / .stp)
STEP (Standard for the Exchange of Product model data) is the universal neutral format for 3D solid models. It is the correct choice for virtually all CNC machining submissions where the part has any three-dimensional complexity.
A STEP file contains the complete 3D solid geometry — surfaces, volumes, and feature relationships — without being tied to any specific CAD software. The machinist can open it in their CAM (computer-aided manufacturing) software, inspect it from all angles, verify feature dimensions, and program toolpaths directly from the solid model.
Use STEP for: All 3D machined parts — milled parts, turned parts, complex profiles, multi-feature geometry
AP203 vs AP214: AP214 includes colour and layer information; AP203 is geometry only. Either works for machining. Specify AP214 if colour-coding features to communicate intent is useful.
What STEP does not carry: Tolerances, surface finish callouts, notes, and material specification. These must be provided in a separate 2D drawing or as PDF annotations.
File naming: Use descriptive names that match your drawing part number. 'bracket_v3_final.step' is acceptable. 'untitled.step' is not.
DXF Files (.dxf)
DXF (Drawing Exchange Format) is a 2D vector format — effectively a flat profile. It is the correct format for laser-cut, waterjet-cut, and plasma-cut flat profiles, and for 2D turned part profiles. It is not a substitute for a STEP file for complex 3D milled parts.
Use DXF for: Flat-profile parts (sheet cutting), lathe turned profiles, simple 2D engraving layouts
Scale: DXF files must be at 1:1 scale. Confirm scale is correct before submitting — scaled DXF files are one of the most common submission errors.
Layers: Keep cut profiles on a separate layer from dimension lines, notes, and construction geometry. The machinist programs from the cut layer — mixing layers creates ambiguity.
Closed profiles: All cut profiles must be fully closed polylines. Open profiles cannot be used to define a cut boundary. Check in your CAD software that all polylines are closed before exporting.
Other Formats
IGES (.igs):
An older neutral format, less reliable than STEP for surface geometry. Acceptable if STEP is not available, but STEP is strongly preferred.
Native formats (.f3d, .sldprt, .catpart, etc.):
Do not submit native formats. The machinist may not have your specific software version. Always export to STEP.
STL:
STL is a mesh format used for 3D printing. It does not carry accurate dimensional geometry and is not appropriate for CNC machining submissions.
What Your 2D Drawing Must Include
Even with a perfect STEP file, a 2D drawing (PDF or DXF drawing format) is required for any part with tolerances tighter than general machining tolerances, surface finish requirements, thread callouts, heat treatment requirements, or any feature that cannot be fully defined by geometry alone.
The 2D drawing is the legal document of record. If there is a conflict between the 3D model and the 2D drawing, the drawing governs.
Title block: Part name, part number, revision, material specification, finish specification, date, and drawn-by fields. These are not optional — they are the minimum required to identify the part in your order history.
Orthographic views: Front, top, and right-side views at minimum. Add section views for internal features (holes, pockets, slots) that are not visible in standard views.
Dimensioned correctly: Every feature the machinist needs to produce must have a dimension. Do not leave features implied by the model. If it matters, dimension it.
General tolerance block: Specify the default tolerance for all dimensions not individually toleranced. A typical general tolerance block reads: Linear ±0.1 mm, Angular ±0.5°.
Feature-specific tolerances: Apply tighter tolerances only to features that functionally require them — mating bores, press-fit pins, sealing faces. Every over-specified tolerance adds inspection cost.
Thread callouts: Fully specify all threads: M6×1.0 – 6H for metric, or UNC/UNF designation for inch threads. Specify depth for blind tapped holes.
Datum references: If GD&T callouts are used, all datum references must be fully defined. Floating GD&T callouts without datum references cannot be inspected.
How to Specify Tolerances Correctly
Technical drawing excerpt showing a plastic machined part with correct tolerance annotation — general tolerance block in title block, feature-specific tolerances only on mating bore and pin holes, surface finish symbol on bearing face — annotated with explanatory labels
Tolerance specification is where most CAD submissions for CNC plastic machining fail. The two failure modes are opposite: over-tolerancing (specifying tighter tolerances than the application requires, which drives up cost) and under-tolerancing (leaving critical dimensions with only general tolerances, which allows out-of-spec parts to be accepted).
Process Capability by Operation
3-axis CNC milling, general dimensions: ±0.1 mm standard capability. ±0.05 mm achievable with careful setup.
CNC turning, OD/ID: ±0.05 mm standard. ±0.02 mm achievable for precision turned features.
Drilled holes: ±0.1 mm on position. For tight positional accuracy, specify reaming or boring.
Reamed holes: ±0.02 mm on diameter. Used for press-fit pins and precision locating holes.
Slots and pockets: Width tolerance ±0.05 mm achievable. Depth tolerance ±0.1 mm standard.
Plastic-Specific Tolerance Considerations
Plastics are not metals. They respond to temperature and humidity in ways that metal does not. A Delrin part machined to ±0.02 mm in a 22°C workshop may be outside tolerance at 35°C operating temperature. Nylon absorbs moisture from the air and swells — parts machined to tight tolerances on a dry day may be out of tolerance after 24 hours at ambient humidity.
Delrin (POM): Best dimensional stability of common engineering plastics. Tight tolerances (±0.02 mm) are achievable and maintainable.
Nylon (PA6/PA66): Avoid tolerances tighter than ±0.05 mm on functional dimensions. Moisture absorption causes dimensional change of 0.3–0.8% in the worst case.
HDPE / PP: Soft, thermally sensitive materials. Specify tolerances of ±0.1 mm or looser. Tight tolerances on these materials are rarely maintainable in service.
Acrylic (PMMA): Brittle but dimensionally stable. ±0.05 mm achievable for milled features. Use caution with thin walls and sharp corners — they chip.
PTFE: Very soft and creep-prone. ±0.05 mm achievable on the machine, but parts in service under compression will deform.
For a full breakdown of tolerance capability by material and operation in our machine shop, see our CNC plastic machining services page.
Surface Finish Callouts Your Machinist Can Act On
Surface finish is specified using Ra (roughness average) — the average deviation of the surface profile from the mean line. Lower Ra = smoother surface = more machining time.
Ra 3.2 μm (125 μin): Standard milled finish. Visible tool marks. Appropriate for structural faces, non-mating surfaces, and general enclosures.
Ra 1.6 μm (63 μin): Fine milled finish. Light tool marks visible. Appropriate for mating faces, low-friction sliding surfaces, and general sealing faces.
Ra 0.8 μm (32 μin): Very fine finish. Requires lighter passes and more time. Appropriate for precision bearing faces, optical mounting surfaces, and tight-sealing faces.
Ra 0.4 μm (16 μin) and below: Requires hand polishing or lapping after machining. Specify only where optically or tribologically required.
As-machined (unspecified): If no surface finish is called out, the machinist will produce a standard milled finish equivalent to approximately Ra 3.2 μm.
Specify surface finish only on faces where it matters functionally. Applying Ra 0.8 μm to all faces of a structural bracket wastes machining time. Apply it to the bearing bore. Leave everything else as-machined.
Material Specification: What to Write and What to Avoid
Material specification on the drawing must be specific enough to be unambiguous and achievable. Common under-specification problems:
'Plastic' or 'nylon': Not a specification. There are dozens of nylon grades with significantly different properties. Specify the grade: PA6, PA66, PA6-GF30 (glass-filled), PA12, etc.
'Delrin': Delrin is a DuPont brand name for POM-H (homopolymer acetal). Acceptable as a specification — most machinists stock it. If you are indifferent between POM-H and POM-C (copolymer acetal), write 'Acetal (POM-H or POM-C acceptable)' to allow substitution.
'Engineering plastic': Meaningless as a specification. Specify the actual material and grade.
Colour specification: If colour matters (for visual identification or aesthetics), specify it. Most engineering plastics are available in natural (off-white/grey), black, and occasionally other colours. Natural vs black is a different material order and different stock.
Food-grade / medical-grade: If regulatory compliance is required, specify the standard: FDA 21 CFR compliant, RoHS compliant, USP Class VI. Material certificates may be required — ask at time of order.
Assembly Files and Multi-Part Submissions
When submitting a multi-part assembly for machining, each part requires its own drawing and its own STEP file. Do not submit assembly STEP files as a substitute for individual part files — the machinist needs to program each part separately.
One drawing per part: Each machined component needs a standalone drawing with its own title block, tolerances, and material specification.
Assembly drawing (optional but useful): An assembly drawing showing how the parts fit together helps the machinist understand context — which faces are mating faces, which dimensions are driven by assembly fit rather than standalone geometry.
Revision control: Use a revision system (Rev A, Rev B, or date-based) and increment it every time the drawing changes. Submitting Rev A and Rev B files with the same part number is a common source of machined-to-wrong-revision errors.
BOM (Bill of Materials): For assemblies of 5 or more parts, include a BOM listing part numbers, quantities, and materials. This prevents missed components in the order.
Mating dimensions: For press fits, slip fits, and clearance fits, specify the fit on both mating parts. Write the fit class (H7/p6 for press fit, H7/g6 for running clearance) rather than calculating and writing individual tolerances — this communicates intent more clearly.
For complex assemblies that combine CNC machining with injection moulded or fabricated components, our product design team can review the full assembly and flag interface issues before machining begins.
The Most Common CAD Submission Mistakes
Submitting an STL instead of a STEP: STL is a mesh format for 3D printing. It does not contain accurate geometry. If your only export option is STL, your CAD software is not the right tool for machined part design.
DXF at wrong scale: A DXF submitted at 1:10 or 1:100 will be machined 10× or 100× smaller or larger than intended. Verify scale at 1:1 before every submission.
Missing surface finish callouts on functional faces: If the bearing bore needs Ra 0.8 μm and it is not specified, it will be machined to as-machined Ra 3.2 μm. The part may technically be in-tolerance on dimension but fail in service.
Tolerances tighter than the material can hold in service: A nylon part machined to ±0.02 mm will absorb moisture after machining and may be outside tolerance by next morning. Match tolerances to material capability in operating conditions.
No revision in the title block: If you submit a revised drawing without changing the revision field, the machinist has no way to know which version they machined last time. Always increment revision.
Conflicting dimensions between 3D model and 2D drawing: If the STEP file shows a 10 mm bore and the drawing dimensions call out 9.5 mm, the machinist must stop and ask for clarification, adding lead time. The drawing governs — keep model and drawing in sync.
Unspecified material: 'Make this in plastic' is not a specification. We stock multiple grades of Delrin, nylon, HDPE, UHMWPE, PTFE, acrylic, polycarbonate, and ABS. Specify which one you need.
Frequently Asked Questions
What file format should I send for CNC machining?
Send a STEP file (.step or .stp) for 3D parts and a DXF file (.dxf) for flat-profile 2D parts. Always send a separate PDF drawing with tolerances, surface finish callouts, and material specification — the 3D model alone is not sufficient for parts with functional requirements.
Can you machine directly from a STEP file without a 2D drawing?
For simple parts with no tight tolerances, no special surface finish requirements, and a clearly specified material, yes. For anything with functional interfaces — mating bores, press fits, sealing faces, threaded inserts — a 2D drawing with explicit callouts is required. When in doubt, include the drawing.
What is the difference between STEP and IGES?
Both are neutral 3D CAD formats. STEP (AP203 or AP214) is the modern standard and is more reliable for complex surfaces and solid geometry. IGES is older and more prone to translation errors on complex geometry. Use STEP wherever possible.
How do I specify a press fit for a plastic part?
Use standard ISO fit codes: H7/p6 for a light press fit, H7/r6 for a heavier press fit. Note that plastic-to-metal press fits behave differently from metal-to-metal — plastic will creep under sustained load. For plastic-to-metal press fits, specify the fit class and note the material combination so the machinist can advise on interference values.
Should I include assembly context when submitting individual parts for machining?
Yes — an assembly drawing or assembly STEP is helpful even when only individual parts are being machined. It tells the machinist which surfaces are mating surfaces, which tolerances are driven by fit rather than standalone function, and what the finished assembly context is. It also helps catch misunderstandings before machining begins rather than after.