How to prepare CAD files for a CNC quote

The short answer

For a CNC machining quote, send two things per part: a 3D model in STEP format (AP203 or AP214, solid body) and a 2D drawing in PDF that carries everything the model cannot: tolerances, thread specifications, surface finish, material and temper, coating, and revision. Add the quantities you want priced and your ship-to country. That is enough for any competent shop to price the part without asking questions.

Most quote delays are not caused by the shop being slow. They are caused by missing information: a mesh file where a solid was needed, a threaded hole with no thread callout, "anodize" without a type or color, or a tolerance block that says ±0.01 mm on every dimension. Each gap costs a day of email back and forth, or worse, gets priced with a guess. The rest of this guide explains each item, then gives you a checklist you can paste into your next RFQ.

What file format for CNC machining? STEP vs STL vs native

CAD files come in two fundamentally different kinds, and the difference matters to the programmer who writes your toolpaths.

B-rep (boundary representation) solids describe the part with exact mathematical surfaces: a hole is a true cylinder with a diameter, a fillet is a true radius, a face is a true plane. STEP, IGES, Parasolid (X_T) and native CAD formats are B-rep. CAM software can select a cylinder and read "Ø6.000 mm", recognize a pocket, and generate a clean toolpath directly from the geometry.

Meshes describe the surface as thousands of flat triangles. STL (and OBJ, 3MF) are meshes. A hole becomes a polygon with, say, 64 facets. The true diameter is gone; it can only be estimated. Fillets become faceted strips. Mesh files were made for 3D printing and visualization, not machining.

Why STEP beats STL for machining

Take a Ø8 H7 bore. In a STEP file it is a cylinder of exactly 8.000 mm. In an STL exported at default resolution it is a polygon whose flats sit inside the true circle and whose corners touch it, so measuring it gives a value somewhat under 8 mm, depending on the chord tolerance used at export. The programmer has to guess the intent, rebuild the feature by hand, or ask you. Multiply that by every hole, boss and fillet on a housing and you see why STL quotes are slower and riskier. Use STL only when the part has no precise features, or when STL is all you have (for example a scanned or sculpted shape), and say so in your notes.

Native files

If your CAD system can export Parasolid, an X_T file is as good as STEP and sometimes cleaner. We accept STEP/STP, IGES/IGS, STL, X_T, DWG, DXF, PDF and ZIP, up to 50 MB each. If you work in a system with an unusual native format, export STEP rather than sending the native file. When exporting, export solids, not surfaces, and check the result in a free viewer: the body should be closed, and the dimensions should match your model.

Technical drawing for CNC machining: what it must show

The 3D model gives the machinist the shape. The 2D technical drawing tells them what matters. It does not need to be a full production drawing with every dimension; for a quote, a "reference + critical features" drawing is enough: the model governs all undimensioned geometry, and the drawing calls out what is tight, threaded, finished or inspected. State this explicitly in a note: "3D model governs all dimensions not shown."

Tolerances: be specific and be selective

A common mistake is a title block that applies ±0.01 mm to everything. That forces slow finishing passes and full inspection on features that do not need it, and it can double the price. Use a general tolerance standard such as ISO 2768-m for the bulk of the part, then call out tight tolerances only on bearing bores, locating pins, mating faces and sealing surfaces. Our standard is ±0.03 mm; tighter tolerances on critical features are available when marked on the drawing and confirmed in the quote. The CNC machining cost guide shows how much tolerance choices drive price.

Material and temper

Write the full designation: 6061-T6, not "aluminum"; 304 or 316, not "stainless"; 4140 annealed or pre-hardened, not "steel". If a grade substitute is acceptable (for example 303 instead of 304 for better machinability), say so; it can shorten lead time and lower cost. If you need a mill certificate, note it on the drawing. Our materials page lists the common grades and their trade-offs.

Finishes and masking

For anodizing, state Type II or Type III, color, and which surfaces must stay bare (threads, bores with H7 fits, grounding points). Anodize adds thickness, so a bore toleranced before coating may go out of tolerance after. Say whether your dimensions apply before or after finishing. Details are in the anodizing guide and on surface finishes.

How to model and call out threads

Do not model helical threads in the 3D file. Modeled threads make the STEP file heavy, confuse feature recognition, and still do not tell the shop the thread class. Instead:

• Model the tap drill or minor diameter for internal threads (for example Ø5.0 mm for M6x1.0) and the major diameter for external threads.
• Use a cosmetic thread in your CAD system so the thread shows on the drawing, but not as real geometry.
• Call out the full specification on the drawing: size, pitch, class and depth. Examples: M6x1.0-6H, thread depth 12, drill depth 15; 1/4-20 UNC-2B ↧ 0.50; M10x1.25-6g for a fine external thread.
• Say if you need inserts: helicoil, threaded inserts or PEM fasteners are separate operations and must be quoted.
• State masking if the part is anodized or plated, so threads are not coated out of gauge.

If a hole on the model has no thread callout on the drawing, a careful shop will ask; a careless one will leave it as a plain hole. Either way it costs time.

Units, assemblies and file naming

Units

STEP files carry a unit, but some exporters scale incorrectly. A 25.4× size error is the classic symptom of inch/mm confusion. State the unit on the drawing and in your RFQ text. If your design is in inches, keep it in inches end to end and give imperial thread callouts; do not mix units within one drawing.

Multiple parts

For a project with several parts, send one STEP and one PDF per part, named identically so they pair up, and put them in a single ZIP:

If you only have an assembly STEP, send it, but list which bodies are to be made and which are purchased (bearings, fasteners) so they are not quoted as machined parts. Avoid names like "final_v2_new.step"; the revision in the file name should match the revision on the drawing.

Which quantities to request

CNC pricing has a large fixed portion (programming, fixturing, first-article setup) and a per-part portion (machine time, material, finishing). Fixed cost is spread over the batch, so unit price falls steeply from 1 to 10 pieces and flattens after that. Ask for two or three quantity breaks in one RFQ so you can see the curve, for example:

• 1 / 5 / 10 for a first prototype
• 10 / 50 / 100 for a pilot build
• 100 / 250 / 500 / 1,000 for low-volume production

Quantity breaks in one request are quick to price; separate requests later take longer. We make parts from 1 piece up to roughly 1,000 pieces. For single prototypes see rapid prototyping.

RFQ checklist for CNC machining (copy and paste)

Paste this into your email or the notes field of the quote form and fill it in. If an item does not apply, write "n/a" so the reader knows it was considered rather than forgotten.

Every order with us includes an inspection report on critical dimensions and first-article approval by photos and measurements before the batch runs; noting what you consider critical makes that report useful. More on this at quality and inspection.

Common mistakes that delay CNC quotes

1. STL only, for a part with precision bores. The shop must reconstruct features or ask for a STEP.
2. No drawing at all. Without one, the quote assumes general tolerances, no threads and as-machined finish, which may not be what you need.
3. Drawing and model disagree. A hole is Ø6 in the model and Ø6.5 on the drawing. State which governs, and check revisions match.
4. Blanket tight tolerances. ±0.01 mm on every dimension inflates cost; quoters will flag it in DFM notes anyway.
5. Unspecified threads. A tapped hole drawn as a plain cylinder, or "M6" with no depth.
6. Vague finish. "Anodized" without type and color, "polished" without a target Ra, "painted" without a RAL code.
7. Sharp internal corners. A milling cutter is round; internal pocket corners need a radius, ideally a bit larger than the cutter radius. Deep pockets with tiny corner radii need long, slow tools.
8. Assembly sent as one body. Merged solids cannot be separated reliably; send individual parts.
9. Missing quantity or destination. Price and shipping cannot be calculated without them.
10. Modeled helical threads and text. Heavy files, slow to load, no added information.