New Product Introduction

What Is a DXF File? And What Makes One Ready to Cut

A DXF is the file most cutting shops ask for. Whether it cuts cleanly on the first try depends on a handful of things you can check before you send it.

Bryan PetroCo-founder, OpenSpindle
Published 8 min read
OPEN GAPDOUBLE LINECUT-READY DXFSCALE 1:1$INSUNITS = 4 (MM)CLOSED CONTOURSONE LINE PER EDGETEXT AS OUTLINESBENDS ON OWN LAYERTHE CUTTER FOLLOWS EVERY LINE IT IS GIVEN, SO GIVE IT ONLY THE PART

The short answer

A DXF file (Drawing Exchange Format) is a 2D vector drawing format created by Autodesk so CAD programs can share geometry. It stores lines, arcs, circles, polylines and splines on named layers, plus a units setting, as either ASCII text or binary. Laser, waterjet, plasma and router shops cut from DXF files. A DXF is cut-ready when it is drawn at 1:1 with units set, every contour is closed, no lines overlap, text is converted to outlines, and dimensions and title blocks are off the cut geometry.

What a DXF file is

DXF stands for Drawing Exchange Format. Autodesk introduced it alongside AutoCAD in the early 1980s so drawings could move between programs, and it became the shared language of 2D CAD. Autodesk publishes the DXF specification, which is why so many programs can read and write it, from full CAD suites to the software that drives a laser cutter.

A DXF can be saved as plain ASCII text or as binary. The ASCII form is human readable: it is a long list of paired lines, a numeric group code followed by a value. The file is split into sections. The two that matter most for cutting are:

  • HEADER, which holds drawing settings, including the units variable $INSUNITS (for example, 1 means inches and 4 means millimeters).
  • ENTITIES, which holds the geometry itself.

Other sections hold layer definitions and blocks (reusable groups of geometry). The DXF format has gone through many releases since R12, and newer releases added entity types: lightweight polylines arrived in R14, and true splines a release earlier, in R13. When a shop asks for an older version such as R12, any splines in your drawing get converted to other geometry on export.

What is inside: entities, layers and units

Everything in a DXF is an entity on a layer.

EntityWhat it isWhat it means for cutting
LINEA straight segment between two pointsCut as drawn
ARC and CIRCLEExact curves defined by center and radiusCut as smooth curves; the preferred way to describe holes and radii
LWPOLYLINE / POLYLINEA chain of connected lines and arcsA closed polyline is the cleanest way to define one cut contour
SPLINEA free-form curveHandled well by some cutting software and poorly by others, which may break it into many short segments
ELLIPSEAn exact ellipseUsually fine; some older software converts it to segments
TEXT / MTEXTText that references a fontNot cut geometry until it is converted to outlines
DIMENSIONA dimension with its arrows and textShould not be on the cut layer
INSERTA reference to a blockSome cutting software ignores blocks, so exploding them is safer

Layers name groups of geometry (for example CUT, ETCH, BEND). Many shops use layers, and sometimes line colors, to tell the machine which operation each line gets.

Vector files vs raster files

A vector file describes geometry mathematically: a line from this point to that point, an arc of this radius about this center. It has no fixed resolution, so it can be scaled to any size without losing accuracy, and every edge has an exact position. DXF, DWG, SVG, AI and EPS are vector formats. A PDF can contain vectors, raster images or both.

A raster file is a grid of pixels: PNG, JPG, BMP, TIFF. An edge in a raster image is only as precise as the pixel size, and it has no notion of a line or a hole, only colored squares.

Cutting machines follow paths, so they need vectors. A laser can engrave a raster image by scanning it line by line, but cutting a part outline needs vector paths. Tracing a raster into vectors is possible, and it is a common source of problems: traced outlines tend to come out as hundreds of tiny wobbly segments instead of clean lines and arcs, at a scale nobody set deliberately. If all you have is an image, plan on redrawing the outline in CAD at real dimensions.

What makes a DXF cut-ready

A laser, waterjet, plasma or router cuts the lines it is given. Every problem below comes from giving it lines that are not the part.

  • Draw at 1:1 and set the units. Draw the part at its real size in millimeters or inches and make sure the file records which. When $INSUNITS is missing, the receiving software has to guess, and an inch part read as millimeters arrives about 25 times too small.
  • Close every contour. Each outline and each hole should be one closed loop. A gap of a fraction of a millimeter stops cutting software from recognizing which side is the part and which is scrap, so it cannot apply kerf compensation or choose lead-ins correctly.
  • One line per edge. Delete duplicate and overlapping lines. A doubled line can be cut twice, which widens the cut, burns the edge and doubles the time on that path.
  • Prefer lines and arcs over splines. Exact arcs cut smoothly. Splines are fine in many systems, but some break them into many short segments that cut slowly and leave a faceted edge. If your CAD offers to export splines as arcs or polylines, ask the shop which it prefers.
  • Convert text to outlines. Text entities depend on a font the shop may not have. Convert text you want cut or engraved to geometry. For cut-through lettering, use a stencil style font, or the centers of letters such as O, A and B fall out.
  • Keep notes off the cut layer. Dimensions, title blocks, borders and notes either go on a separate layer or come out of the file. Material, thickness and quantity belong in the RFQ.
  • Put bend lines on their own layer. For sheet metal flat patterns, bend lines on the cut layer get cut. Label the layer clearly, and note bend direction and angle on a drawing.
  • One part per file, or a clearly separated layout. Several parts in one file is fine if they are clearly separated and you state the quantity of each. Do not nest them tightly yourself: the shop nests for its own sheet size and kerf.
  • Draw nominal geometry. Do not offset the outline for kerf. The shop's cutting software applies kerf compensation for its machine, material and thickness.

Sheet metal: flat pattern DXF or formed model?

A DXF of a flat pattern only works if it was flattened with the same bend allowance the shop will use. The developed length of a bent part depends on material, thickness, inside radius and the shop's tooling, so a flat pattern from your CAD's default settings can produce a part with flanges that come out a little long or short after bending.

For parts that get bent, many shops would rather receive a STEP of the formed part, so they can develop the flat pattern for their own press brake. Send the flat DXF as a reference if you have one, and say which file is the master. The sheet metal DFM guide covers the bend geometry that decides whether a flat pattern forms cleanly.

DXF vs DWG vs STEP vs SVG

These four get confused often because they all hold geometry. They are built for different jobs.

FormatWhat it holdsOpennessUse it for
DXF2D vector geometry on layers (3D is possible but rarely used for cutting)Published by Autodesk, read by nearly all CAD and cutting softwareFlat profiles for laser, waterjet, plasma and router cutting
DWGAutoCAD's native drawing format, 2D and 3DProprietary; other programs read it through licensed or reverse-engineered librariesWorking drawings inside AutoCAD; convert to DXF before sending for cutting unless the shop asks for DWG
STEPExact 3D solid geometry (ISO 10303)International standard (ISO 10303), supported by nearly all 3D CAD3D parts for CNC machining, sheet metal, molding and printing
SVG2D vector graphics for the webOpen W3C standardArtwork and signs; workable for some laser shops, but units default to pixels and scale errors are common

An SVG measured in pixels relies on a pixels-per-inch assumption. The CSS standard uses 96 pixels per inch, but not every program follows it, so an SVG can arrive at the wrong size. A DXF with units set avoids that guesswork.

How to check a DXF before you send it

Open the file somewhere other than the program that made it. The free DXF viewer runs in your browser, and the file stays on your computer unless you choose to request a quote. It reports two numbers worth checking:

  • Overall size. Compare it to the size you designed. If it is off by about 25 times, the units are wrong. If it is off by a small round factor, the drawing was scaled.
  • Total cut length. For a given material and thickness, cutting time depends mainly on cut length and the number of pierces. If the total is far above what the outline suggests, look for a border, a title block, construction lines or doubled lines still in the file.

Then zoom in on corners and hole edges to look for gaps, and turn layers on and off to confirm only the part is on the cut layer. For a 3D part, the STEP viewer does the same job for the solid model.

If you are still choosing a program to draw the part in, free CAD software for parts compares which free tools export clean DXF and STEP files.

Sending a DXF for a quote

With a clean DXF, the rest of the RFQ is short: material, thickness, quantity, finish, and any hole or edge that needs a tighter tolerance than standard cutting holds. Tapped holes, countersinks and bends need a drawing or a note, because a DXF shows a hole's outline but not what happens to it after cutting.

Upload the DXF at /quote with those details. An independent partner shop that runs the process (laser, waterjet, plasma or routing) quotes it, and you get one matched quote, usually in about 24 hours. For the full list of files by process, see what CAD files to send for a manufacturing quote.

Sources

Last reviewed by Tom Petrini

Let us quote your next part.

Upload your CAD or drawing and tell us your budget. We source it across our global network of partner shops and come back with your best-match quote, typically within about 24 hours.

  • Free quote in about 24 hours
  • No minimum order
  • No account needed to start
Add your CAD filesUp to 30 files per quote
Upload files & get a free quote

STEP · STL · IGES · DWG · DXF · SLDPRT · and more

No CAD file? Describe your project instead

Frequently asked questions

What is a DXF file used for?

DXF files carry 2D vector geometry between CAD programs. In manufacturing they are the standard input for laser, waterjet, plasma and CNC router cutting, because cutting software turns the lines and arcs directly into toolpaths.

What is a vector file?

A vector file describes shapes as mathematical geometry, such as lines, arcs and curves with exact coordinates, rather than as pixels. It can be scaled to any size without losing accuracy. DXF, DWG, SVG, AI and EPS are vector formats; PNG and JPG are raster formats.

Can I convert a JPG or PNG into a DXF for cutting?

You can trace one, but the result is usually a cloud of short, uneven segments at an arbitrary scale. For a part that has to fit something, redraw the outline in CAD at real dimensions. Tracing is more workable for decorative artwork where exact size matters less.

What is the difference between DXF and DWG?

DWG is AutoCAD's native, proprietary format. DXF is the exchange format Autodesk publishes so other programs can read and write the same geometry. For cutting, send a DXF unless the shop specifically asks for DWG.

Should I send a DXF or a STEP file for sheet metal?

For a flat part with no bends, a DXF is enough. For a bent part, many shops prefer a STEP of the formed part so they can develop the flat pattern with their own bend allowances. Send the flat DXF as a reference if you have one, and say which file is the master.

Why did my laser cut part come out the wrong size?

The most common cause is units. If the DXF does not record its units, or the file was drawn in inches and read as millimeters (or the reverse), the part scales by about 25 times. Draw at 1:1, set the units, and check the overall size in a viewer before you send it.