What File Format Should You Use for CNC Machine? (A Complete CAD File Guide)

STEP (.step/.stp) is the best file format to use in CNC machines. It stores exact 3D solid geometry, opens cleanly in nearly every CAD and CAM system, and is the format most factories providing CNC machining in China and elsewhere expect to receive.

That doesn't make the other six common formats obsolete. IGES, Parasolid, native CAD files, DXF, DWG, and STL each still have a place in a CNC workflow. The trouble starts when you send the wrong file for the job, or when it arrives without the details a factory needs to provide an accurate factory quote. A DXF with no stated thickness, or an STL sent for a ±0.025 mm feature, leaves the factory with two options: stop and ask, or price in its best guess.

Here's what you actually need to learn what file format to use for CNC machines: how a CAD file becomes G-code, the seven common formats and when to use each, what to send alongside your file for an accurate quote, and the five checks worth running before you upload.

TL;DR / Key Takeaways

• CNC machines run G-code rather than CAD files. A CAM programmer converts the STEP or DXF file into G-code before machining, so a clean CAD file means a faster, more accurate CNC quote.
• CAD formats fall into two groups: neutral formats (STEP, IGES, Parasolid, DXF) open in almost any software, while native files (SLDPRT, IPT, CATPart, PRT, DWG) are proprietary to the program that made them.
• STEP is the best file format for 3D CNC parts and DXF for flat, profile-cut parts. Send IGES only as a fallback and convert any STL to a solid model before CNC machining.
• Always send a 2D drawing with your CAD file - tolerances, GD&T, threads, and surface finish live on the drawing, and it's what the factory prices and inspects against.
• Incomplete CNC RFQs receive higher quotes because a factory that has to guess the material, tolerances, or units prices on the safe side.
   

How does a CAD file become a CNC machining job?

A CAD file becomes a CNC machining job when a CAM programmer converts it into G-code. CNC machines run G-code, a sequence of machine instructions covering tool movements, feed rates, and spindle commands, and cannot read the submitted CAD file directly.

1. CAD - The part's geometry is designed or exported (STEP, IGES, DXF, and so on).
2. CAM - A programmer imports that geometry, defines the machining operations, and builds toolpaths.
3. Post-processing - The toolpaths run through a post-processor tuned to the machine controller (Fanuc, Siemens, and Haas each read slightly different G-code dialects).
4. G-code - The resulting program (a .nc, .tap, or .gcode file) loads onto the machine and runs.

G-code generation from CAD is the factory's job. What the CAM programmer needs is a CAD file that imports as one clean solid, because every gap or missing face adds repair time before the CNC machining workflow can move past step 2, and that time shows up in the quote.

What are the common CAD file formats for CNC machine?

The most common CAD file formats for CNC machining are STEP, IGES, Parasolid, native CAD files, DXF, DWG, and STL. Like image formats (JPEG, PNG, GIF), each was built at a different time for a different job, so each stores geometry differently. That difference decides whether a factory can program your part straight from the file or has to stop and ask questions first.

Most CAD file formats for CNC machining fall into two groups: neutral and native.

• Neutral (universal) formats: such as STEP and IGES are open standards designed to share models between different software. Nearly any CAD or CAM system can read them. They carry the part's final geometry but not how it was modeled.
• Native formats such as SolidWorks (.sldprt), Siemens NX (.prt), and Autodesk Inventor (.ipt) are each CAD program's own file type. They hold more information, including the feature tree, but support outside the original software varies. However, a supplier's CAM system may not read your file, or may not read the version you saved it in.

Uploading a native file the supplier can't open is a common reason an RFQ stalls. Most CAD programs can export a neutral format such as STEP, so sending a STEP file together with a 2D PDF drawing avoids the problem.

Format	Extension	Native / Neutral	Geometry	Compatibility
STEP	.step, .stp	Neutral (ISO 10303)	Exact 3D solid; newer versions can also carry tolerances and other drawing data	Opens in nearly all CAD/CAM software; the default choice for CNC RFQs
IGES	.iges, .igs	Neutral (old US standard, not updated since 1996)	3D surfaces and curves; solids often arrive as loose surfaces that need repair	Widely readable, but surface gaps slow programming; use as a fallback
Parasolid	.x_t, .x_b	Neutral (owned by Siemens)	Exact 3D solid	Reads cleanly in most CAD/CAM software; newer versions may not open in older software
SLDPRT	.sldprt	Native (SolidWorks)	Exact 3D solid plus the full feature tree	Best in SolidWorks and its built-in CAM; not readable by older SolidWorks versions; support elsewhere varies
DXF	.dxf	Neutral (openly published by Autodesk)	Mostly 2D lines, arcs, and outlines; no thickness or depth	Universal for flat parts (laser, waterjet, sheet metal); not enough on its own for 3D machined parts
DWG	.dwg	Native (AutoCAD)	2D drawings (can hold basic 3D, but rarely used that way)	AutoCAD and most CAD programs; useful as a drawing, not as a 3D model for machining
STL	.stl	Neutral (developed for 3D printing)	Triangle mesh; no true curves, units, or tolerances	Opens almost anywhere, but a mesh can't hold CNC-level accuracy; avoid for machining quotes

STEP (.step/.stp)

STEP (Standard for the Exchange of Product Data, ISO 10303) is the default format for CNC quotes. It stores exact solid and surface geometry, so a factory running SolidWorks can open a STEP file exported from Fusion 360, Inventor, or Creo without the model breaking during translation.

STEP comes in several versions, called application protocols (APs). Your CAD software asks you to pick one when exporting:

Protocol	What it carries	When to use it
AP203 (1994; Edition 2 in 2011)	Solid geometry and assembly structure; the original edition carries no color, layers, or PMI	Legacy systems; fine for simple parts
AP214	Adds color and layer data; developed for automotive workflows	General-purpose export
AP242	Merges AP203 and AP214; supports Model-Based Definition (MBD), meaning GD&T, tolerances, and other PMI stored inside the 3D model	Tolerance-critical parts, especially aerospace and medical

PMI (product and manufacturing information) is the tolerance, GD&T, and surface finish data that normally sits on the 2D drawing. Any STEP version works for a standard CNC quote. When tolerances need to travel inside the model, export as STEP AP242 rather than the default setting.

STEP AP242 does not guarantee that a factory reads the stored tolerances. The factory's CAM and inspection software has to support PMI on import, and NIST's PMI conformance testing found gaps in how major CAD systems handle PMI in STEP files. Many CNC shops open a STEP AP242 file, use the geometry, and ignore the stored tolerances. The safe default is to send a 2D PDF drawing with the STEP AP242 model unless the supplier confirms it reads embedded PMI.

IGES (.iges/.igs)

IGES (Initial Graphics Exchange Specification) is an older neutral format, first published in 1980 by the US National Bureau of Standards. It's still in use, mostly for legacy data and surface-heavy models. It transfers wireframes and surfaces reliably, but although later versions can describe solids, most IGES exports still arrive as separate surface patches rather than one closed solid.

That's its practical weakness. A complex model can arrive as loose surfaces with tiny gaps at the seams. A CAM programmer then has to “heal” the surfaces before generating toolpaths, which is billable time a clean STEP export avoids. IGES files also tend to be larger than the equivalent STEP file.

STEP vs IGES: STEP describes a part as a solid and is the safer default. IGES is older, usually arrives as surfaces, and is more likely to have gaps. For a new 3D model going out for a CNC quote, send STEP.

Parasolid (.x_t/.x_b)

Parasolid is the geometric modeling engine (kernel) behind SolidWorks, Siemens NX, Solid Edge, and Onshape, and it can also be saved as a file. .x_t is the text version, easier to inspect and send; .x_b is binary and more compact. Like STEP, it carries exact solid geometry without feature history. Because many CAD and CAM systems run on the same kernel, Parasolid files often import with very high fidelity and load quickly.

Parasolid is a strong choice when you know the factory uses Parasolid-based software. When the supplier's CAD/CAM setup is unknown, STEP is still the safer default.

Native CAD files (SLDPRT, IPT, CATPart, PRT)

Native files are the format each CAD program saves in by default: SolidWorks (.sldprt), Autodesk Inventor (.ipt), CATIA (.CATPart), and Siemens NX and PTC Creo (.prt). They carry more information than any other format - full feature history, sketches, parametric constraints, and design intent, not just the finished geometry.

That depth has two costs:

• Compatibility. A native file depends on the software, and often the exact version, it was made in. A factory without the same setup may not be able to open it.
• Exposure. A native file reveals the design history and construction logic that a neutral export like STEP leaves out, which matters for protecting your IP.

For most CNC RFQs, export to STEP and send the native file only if the factory asks for it.

DXF (.dxf)

DXF is an exchange format made for moving 2D data between CAD and CAM software. It's the standard for flat, profile-based work: laser, waterjet, and plasma cutting, CNC punching, and 2.5D routing.

A DXF describes shape only. It doesn't state material, thickness, or finish. A common, avoidable mistake is sending a clean DXF profile with no material grade or plate thickness, which forces the factory to stop and ask before it can price the stock.

DWG (.dwg)

DWG is AutoCAD's native drawing format. Like DXF, it comes from AutoCAD and handles 2D geometry. It also carries richer data such as layers, blocks, and annotations. But it's proprietary and less widely supported in CAM software, so it works better as a reference drawing than as a file to cut from. Like a DXF, it doesn't state material, thickness, or finish on its own.

DXF vs DWG for CNC machining:

Feature	DXF	DWG
Type	Neutral (openly published by Autodesk)	Native (AutoCAD)
Best use	2D CAD/CAM data exchange	Detailed 2D drawings, layouts, annotations
Common geometry	Lines, arcs, circles, splines	Same, plus richer CAD metadata
CNC use case	Laser, waterjet, plasma, punching, profile cutting	2D CNC work, if the CAM software supports it
CAM compatibility	Broad, near-universal	Narrower; depends on the receiving software
Typical failure mode	Missing thickness or material	Version or layer mismatch on import

STL (.stl)

STL isn't suitable for precision CNC machining, and it's one of the most common file-format mistakes buyers make. An STL describes a part as a mesh of flat triangles rather than a true solid. Curved surfaces are approximated, precise arcs become chains of short straight segments, and no tolerance or GD&T data survives the export.

STL was built for 3D printing, organic shapes, and scanned parts, where a mesh is the natural way to describe the shape. A machined part with functional tolerances needs a solid model, such as a STEP or Parasolid file exported from the original CAD model, because a mesh can't drive an accurate toolpath around a precise feature. For a fuller comparison of the two processes, see CNC machining vs 3D printing.

The STL to solid conversion process for CNC machining takes five steps. To convert an STL to a solid model:

1. Import the STL as a mesh. Fusion 360, SolidWorks, and FreeCAD each have a mesh-import tool separate from solid modeling.
2. Repair the mesh. Fix non-manifold edges, flipped normals, and gaps, because a damaged mesh produces a damaged solid.
3. Convert the mesh to a solid (B-rep). Use Fusion 360's Mesh to BRep, SolidWorks ScanTo3D (SolidWorks Premium), or FreeCAD's Part workbench (Create shape from mesh).
4. Rebuild critical features by hand. Holes, pockets, and precise radii rarely convert cleanly and usually need redrawing.
5. Export as STEP once the model is a watertight solid rather than a solid-looking mesh.

A STEP file converted from an STL is a draft for review, not a finished submission. The accuracy of the converted STEP file depends on how fine the original mesh was.

Which is the best file format for CNC machining?

The best file format for CNC machining is STEP for most 3D parts and DXF for flat, profile-cut parts, while STL only becomes usable once it's converted to a solid. Across all seven formats, the choice comes down to three questions:

1. Does the file carry true solid geometry, or just an approximation?
2. Will a CAM programmer need to repair anything on import?
3. Does it tell the factory everything needed to machine the part, or does it still need a 2D drawing alongside it?

Format	True solid geometry?	Repair needed on import?	Needs a 2D drawing?	Best for
STEP (.step/.stp)	Yes	Rarely	Yes, unless the factory confirms it reads AP242 PMI	Most 3D machined parts
IGES (.iges/.igs)	Usually surfaces only	Often; surface gaps need healing	Yes	Legacy or surface-heavy data
Parasolid (.x_t/.x_b)	Yes	Rarely; older software may not open newer versions	Yes	Factories using Parasolid-based software
Native (SLDPRT, IPT, CATPart, PRT)	Yes, plus feature history	None, but it opens only if the factory has the same software and version	Yes	In-house edits; send only on request
DXF (.dxf)	No; 2D outlines only	Sometimes (unit errors, open outlines)	Not always, but material and thickness must be stated in the RFQ	Flat and profile-cut parts
DWG (.dwg)	No; 2D drawing	Depends on the factory's CAM support	It often is the drawing; material and thickness still need stating	Detailed 2D drawings
STL (.stl)	No; mesh approximation	Yes; must be rebuilt as a solid	Yes	3D printing and scanned shapes, not CNC

In practice, the decision is simple. For a 3D part, send a STEP file with a 2D PDF drawing. For a flat, profile-cut part, send a DXF and state the material and thickness in the RFQ. For anything else, convert it first or check with the factory before you send it.

What is the best file format for CNC machining?

STEP is the best file format for CNC machining and the most common file format cnc machining factories receive, because it carries exact solid geometry that nearly every CAD and CAM system opens without repair. Which format fits a specific CNC part still depends on its shape, how tightly it is toleranced, and which files already exist.

The most common file format for CNC machining cases:

• Standard 3D machined parts (housings, brackets, milled or turned components): STEP with a 2D PDF drawing. If your tolerances are defined digitally in the model, as is common in aerospace and medical work, use STEP AP242 and still include the drawing.
• Flat, profile-cut parts (plate brackets, panels, sheet-metal blanks): DXF, with the material and thickness stated in the RFQ. If the part is bent after cutting, send a STEP file of the formed part as well.
• Assemblies: One STEP file for each part to be machined, plus the full assembly for reference.
• Parts with only older files or a 2D drawing: IGES or a PDF drawing can still be quoted, but the factory will need to repair surfaces or build the 3D model, which adds time. Re-export to STEP if the original model still exists.
• Mesh-only or scanned parts: Convert the STL to a solid model and send it as STEP.

A factory running a specific CAD/CAM setup (Parasolid, for instance) may ask for that format, or for your native file if it needs to modify the design. Without a stated preference, STEP is the fastest route to a complete, comparable CNC factory quote.

File formats by CNC process

The CNC process your part goes through also affects which file to send.

• CNC milling: STEP, with a 2D drawing. Milling removes material in three dimensions, so the factory needs a true solid model to program toolpaths. Simple 2.5D parts, such as flat plates with pockets and holes, can sometimes be milled from a DXF, but only if the drawing states every depth.
• CNC routing: DXF or DWG for 2D and 2.5D work such as sign panels, cabinet parts, and cut-out shapes. For 3D router work, send STEP for precise parts. STL is common only for decorative carving and reliefs, where tight tolerances don't matter.
• CNC plasma cutting: DXF, drawn at 1:1 scale with closed outlines. Plasma follows a 2D profile through the plate, so state the material and plate thickness in the RFQ. Holes smaller than the plate thickness rarely cut cleanly with plasma and are usually drilled afterward.
• Laser, waterjet, and plasma cutting: DXF is the standard for all three. Keep only the cut geometry in the file, with no title block, dimensions, or notes on the cutting layer, close every outline, and list the material and thickness separately. See our guide to sheet metal fabrication techniques for more on each process.

Process	File to send	State in the RFQ	Watch out for
CNC milling	STEP + 2D drawing	Material, tolerances, finish	DXF only for simple 2.5D plates
CNC routing	DXF/DWG (2D); STEP (3D)	Material, sheet thickness	STL only for decorative carving
CNC plasma cutting	DXF, 1:1 scale	Material, plate thickness	Holes smaller than plate thickness
Laser and waterjet cutting	DXF, cut geometry only	Material, thickness	Open outlines, extra notes on cut layer

How to prepare a CAD file before uploading it?

Preparing a CAD file for an RFQ comes down to five checks: model geometry, units, export format, drawing-to-model match, and which document governs. Together, they catch the problems that most often stall a quote or produce the wrong part.

• Step 1: Check the model geometry. Before exporting, confirm your model is one closed solid with no gaps, missing faces, duplicate bodies, or leftover construction geometry. Your CAD program's geometry-check tool flags gaps and missing faces; check the body list for duplicates and hide construction geometry before exporting.
• Step 2: Confirm units and scale. A millimetre/inch mix-up can scale the part by 25.4 times. STL has no units and many CAM systems ignore DXF units, so measure one known feature and state the units on the RFQ.
• Step 3: Export the right format. Export most CNC parts as STEP (AP214, or AP242 if you include PMI), one part per file, with any assembly added only as a reference. Use Parasolid or DXF when the format table above calls for it.
• Step 4: Match the drawing to the model. Make sure your 2D drawing and 3D model show the same revision, with matching dimensions, holes, threads, and GD&T. Put the part number and revision in the title block and both filenames (for example, 1042-Bracket_RevC.step and 1042-Bracket_RevC.pdf).
• Step 5: State which document governs. Add a note to your drawing stating which document governs if the drawing and 3D model conflict. The drawing usually governs, but with a STEP AP242 file carrying PMI, the model may. Decide whether the drawing or the model takes precedence before you send the file.

Once all five checks pass, put the STEP file, the PDF drawing, and any reference files into a single ZIP with matching filenames.

What are the CAD file requirements for a CNC machining quote?

The CAD file requirements for a CNC machining quote come down to three things: the 3D CAD model, a 2D engineering drawing, and the manufacturing specifications. The file format shows a factory the part's shape, but only all three together tell it exactly what to make and how to price it.

What to include with a CAD file for an accurate CNC quote:

1. 3D CAD model: The part's geometry, sent as STEP (or Parasolid if the factory uses Parasolid-based software)
2. 2D engineering drawing: Tolerances, GD&T symbols, threads, and surface finish, sent as a PDF that shows the same revision as the model
3. Manufacturing specifications: Material, quantity, finish, and quality requirements, listed in the RFQ

The specifications are the easiest part to leave out, because the 3D model doesn't carry them and the drawing rarely covers all of them. The information needed for a CNC quote beyond the file itself is listed below:

Requirement	What to specify
Material	Full grade and temper, not just the family (6061-T6, not just “aluminium”)
Quantity	Prototype quantity and expected production volume, if known
Tolerances	Critical dimensions with their tolerances; on metric drawings, general tolerance per ISO 2768 is a reasonable default for everything else
Surface finish	A stated Ra value (for example, Ra 1.6 µm) or finish type, not just “smooth”
Secondary processes	Anodising, plating, heat treatment, passivation, each called out with its own spec
Inspection & documents	Inspection reports (such as CMM or first article) and material certificates, if required
Supplier certification	ISO 9001, IATF 16949 (automotive), AS9100 (aerospace), or ISO 13485 (medical), if your industry requires it
Lead time	Target delivery date and shipping destination

The fastest way to send all of this is through Haizol's Quick RFQ form.

Enter your Product Quantity and pick a Material. Then add anything the drawing doesn't cover under Special Requirements.

Toggle on Advanced Options to unlock five more fields: NDA, Material Grade, Surface Roughness, Tolerance Requirements, and Secondary Process. Each one shows an example format, so type it the same way (e.g., 6061-T6, Ra 1.6, +/-0.02 mm).

Finally, click Upload Design File and attach your STEP file and PDF drawing. CAD, PDF, ZIP/RAR, and image files are accepted, up to 200 MB each.

Here's what that looks like:

Double-check that what you entered matches the drawing's title block, then hit Continue to Get Quotations.

A Haizol key account manager reviews the RFQ for completeness before any factory sees it. Every factory quotes from the same file, drawing, and specs, so the quotes are easy to compare side by side. From there, price comes down to machine time, setups, tolerances, and finishing. Our CNC machining cost guide breaks down each one.

Frequently Asked Questions

What file format do CNC machines actually use?

CNC machines execute G-code: machine-readable instructions for tool movement, feed rate, and spindle control. The machine doesn't read the CAD file a buyer sends. A CAM programmer uses it to generate the G-code the machine runs.

What is the best file format for CNC machining?

STEP (.step/.stp) is the best default for most 3D CNC-machined parts. It preserves true solid geometry and is supported by nearly every CAD and CAM system, making it the safest choice when you don't know the factory's software in advance.

Can you use an STL file for CNC machining?

Not directly for tolerance-critical geometry. STL stores a part as a triangulated mesh, so curved surfaces are approximated and no tolerance data survives the export. STL suits 3D printing and scanned or organic shapes. For a machined part with functional tolerances, send STEP or Parasolid instead, or convert the STL to a solid first.

Is DXF suitable for CNC machining?

Yes, for 2D and flat-profile work such as laser cutting, waterjet cutting, and CNC punching. A DXF file describes only an outline, so you must specify material and thickness separately.

Which is better for 2D CNC work, DXF or DWG?

DXF is the more universal choice: an exchange format supported by nearly all CAM software. DWG carries richer design data, but it's proprietary to AutoCAD and less consistently supported.

What is the difference between STEP AP203, AP214, and AP242?

The original AP203 carries solid geometry only (Edition 2 added color, layers, and some PMI). AP214 adds color and layer information. AP242, the current and most complete version, supports full Model-Based Definition, so GD&T and other manufacturing data can be embedded directly in the 3D model.

Do I still need a 2D drawing if I already have a 3D CAD model?

A 2D drawing is still needed alongside a 3D CAD model for any part with functional tolerances, thread specifications, or a required surface finish. A 3D model defines nominal geometry only, so tolerances and inspection requirements need an accompanying drawing unless they're embedded as PMI in a format like STEP AP242.

You know the right file format - here's where to send it

Format is settled fast: STEP for most 3D parts, DXF for flat profile work, STL only once it's converted to a solid. That decision alone doesn't get you a quote, though. The drawing, material grade, tolerance class, and finish requirements are what turn a CAD file into a quote that doesn't need a follow-up email.

If you're sourcing CNC machined or sheet metal parts, submit a complete STEP-plus-drawing package on Haizol and the file gets reviewed for completeness before it reaches any factory. That's the difference between an accurate quote the first time and one that needs several rounds of clarification.