Every laser, plasma, waterjet and CNC router shop asks for the same thing: "Send me a DXF." A good DXF cuts first time. A bad one opens at the wrong size, cuts lines twice or will not cut at all. This guide explains what makes a DXF ready to cut, and shows you how to make one with three free browser tools.

What Is a DXF and Why Do Cutters Want It?

DXF stands for Drawing Exchange Format. Autodesk created it so that different CAD programs could swap drawings. It is a plain text file. It lists simple shapes such as lines, arcs, circles and polylines, each with exact coordinates.

That is exactly what a profile cutter needs. A laser or plasma table does not care about colours, title blocks or 3D solids. It needs the path the torch or beam must follow. The CAM or nesting program reads the DXF, finds each closed shape, decides what is inside and outside, adds kerf compensation and lead-ins, and writes the machine code.

Nearly every CAM and cutting package can import a DXF. That is why it is the common language between the person who designs a part and the shop that cuts it.

What Makes a Good Cutting DXF

A DXF can look perfect on screen and still cause trouble at the machine. Check these points before you send a file.

Closed outlines

Each part outline and each hole must be a closed loop. The CAM program uses closed loops to tell the outside of a part from a hole. If two ends miss each other by even a tiny gap, the software may refuse the shape or cut it on the wrong side.

No duplicate or overlapping lines

A line drawn twice gets cut twice. On plasma that burns the edge. On any machine it wastes time. Overlapping lines can also confuse the software when it tries to join shapes into loops.

True arcs, not hundreds of tiny segments

A circle stored as a real arc or circle cuts smoothly. A circle made of 200 short lines makes the machine slow down at every joint, and it can leave a faceted edge. Use true arcs wherever the shape really is round.

Correct units and scale

Draw at full size, 1:1. A DXF stores numbers, and the header variable $INSUNITS says whether those numbers are millimetres or inches. Some programs ignore it and ask you instead, so always check a known dimension after import.

R12 compatibility

Newer DXF versions hold features that older cutting software cannot read. R12 (AC1009) is the oldest common version and the safest choice. All three tools in this guide write R12.

Sensible layers and origin

Put cut geometry on clear layers, such as outlines on one layer and holes on another. Keep construction lines, centre marks and dimensions off the cut layers, or leave them out. Put the origin (0,0) somewhere sensible, usually the bottom-left corner or the centre of the part.

No text or splines unless converted

Text in a DXF is just a font reference, not a path. Most cutting software cannot cut it until it is turned into outlines. Splines and ellipses are also poorly supported by older software. Convert them to lines and arcs in your CAD program before you export.

Closed loops: good Open gap: will not cut Duplicate edge: cut twice Each part and each hole should be one clean, closed loop.
Closed, single loops are what CAM software expects.

Choosing the Right Free DXF Tool

Machinist Central has three free tools for making cutting files, and a fourth that prices them. They all run in your browser and nothing is uploaded. Pick the one that matches your starting point.

You have... Use this tool What you get
A standard part: plate with holes, flange, gasket, gear, sprocket, washer or shim DXF Part Maker Type a few sizes and get a checked part with true arcs, on layers OUTLINE, HOLES and an optional CENTER layer
A custom shape you can dimension DXF Sketcher A small 2D CAD program with typed coordinates, snaps, fillets and edit tools
An existing drawing, scan, template or logo Image to DXF Converter Traced closed outlines with holes, scaled to real size
A finished DXF that you need to quote or check DXF Cut Cost Estimator Cut length, pierces, holes, part area and machine time, with a price per part and per batch for laser, plasma, waterjet or router

The tools also work together. You can open a file from the Part Maker or the Image to DXF Converter in the Sketcher with Import DXF, add a cut-out or extra hole, and export it again. Then drop the finished file into the Cut Cost Estimator to see what it will cost to cut.

Worked Example 1: A Spur Gear or Sprocket in the DXF Part Maker

The free DXF Part Maker draws common flat parts from a few numbers. It makes plates and brackets with hole grids, bolt circles and slots; ASME B16.5 Class 150 and EN 1092-1 PN16 flanges and gaskets; involute spur gears by module or diametral pitch; ANSI B29.1 (#25 to #80) and ISO 606 (06B to 16B) chain sprockets; washers and shims; and bores with DIN 6885 or ANSI B17.1 keyways.

Steps: a module 2, 20-tooth gear

  1. Open the DXF Part Maker and choose Spur gear as the part type.
  2. Set Units to Millimetres. Enter your Material thickness so the checks can warn about small holes and thin webs.
  3. Set Tooth size by to Module, then enter module 2, 20 teeth and a 20° pressure angle. Leave profile shift at 0.
  4. Add a Backlash allowance if you want one. The tool suggests a total of 0.04 to 0.1 × module, split between the two gears.
  5. Enter the bore diameter and pick a keyway standard, or None.
  6. Check the live preview and the checks panel, then click Download DXF.

For this gear the tool gives a pitch diameter of 2 × 20 = 40 mm, an outside diameter of 44 mm and a root diameter of 35 mm. The tooth flanks are true involutes, made by rolling a standard rack around the gear the way a hob cuts it. The flanks are written as short lines that stay within 0.002 mm of the true curve. The tip and root are true arcs.

Small gears and undercut

Below about 17 teeth at 20° a standard rack cuts away the bottom of the tooth flank. The Part Maker warns you and tells you how much positive profile shift fixes it. For example, at 10 teeth it suggests a shift of 0.42. You can also use a 25° pressure angle or more teeth. A shifted gear has a larger outside diameter, so the centre distance or mating gear must suit.

Doing a sprocket instead

Choose Sprocket, pick the chain, and enter the number of teeth. For #40 chain (0.500 in pitch, 0.312 in roller) and 20 teeth, the pitch diameter is 3.1962 in and the outside diameter is 3.4569 in. The teeth follow the ANSI B29.1 tooth form and are drawn as true arcs.

Why the Part Maker files cut well

  • Each outline is a single closed polyline, with true arcs on round edges. Holes are circles.
  • Holes and slots are checked. A hole outside the material or touching another cut shows an error, and the download waits until you fix it.
  • The Origin (0,0) option lets you put zero at the centre or the bottom-left of the part.
  • If your software does not like polylines with arcs, set Outline entities to Separate LINE and ARC entities.
  • The CENTER layer (centre marks, bolt and pitch circles) is left out unless you switch it on, so it cannot be cut by mistake.

Flange or plate hole positions can be cross-checked with the Bolt Circle Calculator.

Worked Example 2: A Plate With Corner Radii in the DXF Sketcher

When the part is not a standard shape, draw it in the online DXF Sketcher. It has lines, rectangles, circles, arcs, slots and polygons, plus fillets, move, copy, rotate, mirror and offset. It also has snaps to ends, middles, centres, quadrants and intersections, and layers.

The key to exact parts is typed input. While a tool is active, start typing and the numbers go into the box at the bottom of the drawing. Use Tab to move between boxes and Enter to apply.

  • 30,15 is the absolute point X 30, Y 15.
  • @40,0 is 40 to the right of the last point.
  • @50<30 is 50 long at 30°, measured counter-clockwise from +X.
100 mm 60 mm 4 × Ø8 R10 corners hole centres 10 mm from each edge
The target part: 100 × 60 mm, R10 corners, four Ø8 holes.

Steps: 100 × 60 mm plate, R10 corners, four Ø8 holes

  1. Set the units to mm. Press R for Rectangle, type 0,0 and press Enter for the first corner.
  2. Type 100, press Tab, type 60 and press Enter. You now have four lines.
  3. Press F for Fillet, type 10 in the Radius box and press Enter. Click the two lines at each corner in turn. The long edges shrink to 80 mm and the short ones to 40 mm.
  4. Make HOLES the current layer. Press C for Circle, type 10,10 and press Enter for the centre. Tab to Diameter, type 8 and press Enter.
  5. Repeat at 90,10, 90,50 and 10,50. Or select the hole and use Copy (K) with @80,0.
  6. Check the size box. It should show 100 × 60 mm, 1 closed outline and no open ends. Click DXF.

The file holds one closed POLYLINE on layer OUTLINE, with four true 90° arcs at the corners, and four circles of radius 4 on layer HOLES. Each hole sits on the centre of its corner radius, which leaves 6 mm of material all round. The outline is 302.8 mm of cut.

A few Sketcher habits that save trouble at the machine:

  • Snap to ends when you draw, so lines really meet. Open ends show as red circles.
  • If the size box reports duplicates, click Delete duplicates.
  • Put layout lines on the CONSTRUCTION layer. They stay out of the DXF unless you tick the box to include them.
  • Tick Move the lower-left corner to 0,0 if you want a clean origin.
  • The export is R12 with $INSUNITS set to mm or inches.

Worked Example 3: Tracing a Logo or Scanned Gasket With Image to DXF

Sometimes all you have is a paper template, an old gasket or a logo. The Image to DXF Converter turns a scan, photo or sketch into vector shapes. It makes the image black and white, traces the shapes, tidies the lines and scales them to real units.

Steps: trace a gasket and set its real size

  1. Scan the gasket or template on a flatbed scanner if you can. A scan has no perspective. If you must use a photo, take it square on in even light.
  2. Click, drop or paste the image into the converter.
  3. Choose Outline mode. It traces every filled shape as a closed loop, and each hole gets its own loop. A gasket gives an outer outline and its bolt holes and bore.
  4. Leave Auto (Otsu) threshold on for a clean scan. For a photo with shadows, try Photo mode. Check the B&W view: the shape should be solid and the background clean.
  5. Raise Ignore specks to drop dust, or use Crop to trace only the part you need.
  6. Turn on Fit arcs (beta) so round holes and curves become true arcs and circles.
  7. Under Set size by, choose Measuring two points. Click Pick two points on the preview, then click both ends of a feature you know. A good choice is the distance between two bolt hole edges, or the full outside diameter. Type the real distance.
  8. Pick the units and the origin (bottom-left or centre), click Trace Vectors, check the size box, and click Download DXF.

The DXF uses layers OUTER for outside edges and HOLES for holes. Centreline mode, which puts pen strokes on a LINES layer, is for line drawings. Its single open lines suit engraving or scribing, not profile cutting, so use Outline mode for anything you want to cut out.

For a logo, the same steps apply. Letters with closed counters, like O and A, come out with their inner holes. You can also use the converter for lettering: print the text in a bold font, then trace it as an outline. That avoids the text problem described above.

Traced shapes are approximations

The tracer follows pixel edges, so accuracy depends on the scan resolution. The converter does not correct a photo taken at an angle. Always measure a known dimension in CAD before you cut. For a part that must fit, use the trace as a guide and redraw the critical holes to exact size in the DXF Sketcher.

Worked Example 4: Estimating the Cutting Cost

Once the DXF is ready, the DXF Cut Cost Estimator tells you what it will take to cut. It measures the cut length, counts the pierces, finds the outer profile and the holes, and works out the part area. Then it turns your cutting speed and shop rates into a price. It also flags open outlines, duplicate lines and holes that are too small for the thickness.

Steps: price 50 brackets in 3 mm mild steel on a fibre laser

  1. Open the estimator and click Try an example. It loads a 120 × 80 mm plate with R10 corners, four Ø10 holes and a 40 × 10 mm slot. Or drop in your own DXF.
  2. Check the layers. Centre lines and text start unticked, so only the outline, holes and slot count.
  3. Choose Fibre laser, Mild steel, 3 mm and a quantity of 50. The typical speed fills in as 3,600 mm/min with 0.3 s per pierce. Type your own machine's speed if you know it.
  4. Enter your shop rates. This example uses 120 per hour plus 10 per hour for gas, 15 minutes setup, 0.25 minutes handling per part, steel at 1.20 per kg with 25% scrap, 20% markup and a 50.00 minimum charge.

The estimator measures 599.91 mm of cut and 6 pierces: the outline is 382.83 mm, the holes 125.66 mm and the slot 91.42 mm. The part area is 8,821.46 mm².

  • Time: 599.91 ÷ 3,600 = 10.0 s of cutting, 6 × 0.3 = 1.8 s of piercing and 15 s of handling, so 26.8 s per part.
  • Machine: 11.8 s of beam time at 130 per hour, plus handling at 120 per hour, = 0.93 per part.
  • Setup: 15 minutes at 120 per hour = 30.00, or 0.60 per part over 50.
  • Material: 8,821.46 mm² × 3 mm × 7.85 g/cm³ = 0.208 kg, plus 25% scrap = 0.260 kg, so 0.31 per part.
  • Price: 1.84 subtotal plus 20% markup = 2.21 per part, or 110.26 for 50.

A single part would work out at 37.49, so the 50.00 minimum charge applies. On a small part like this, handling and setup cost more than the cutting. On thick plate, cutting and piercing take over. You can copy the result as text, download it as CSV or print it.

The speeds are starting values

The built-in speeds are typical figures for a 3 kW fibre laser, a 4 kW CO2 laser, 45 to 105 A air plasma, a 60,000 psi abrasive waterjet and a 6 mm router cutter. Your machine may be quite a bit faster or slower. Time a test cut and use your own speed for real quotes.

Cutting Tips: Kerf, Lead-ins, Hole Sizes and Nesting

Leave kerf to the CAM

Kerf is the width of material the beam, arc, jet or cutter removes. Draw the finished part size. Let your CAM or cutting software apply kerf compensation, outside the outline and inside the holes. If you add kerf to the drawing as well, the part ends up wrong by a full kerf.

Typical kerf is 0.1 to 0.3 mm on a fibre laser, 1 to 2 mm on plasma and about 0.8 to 1 mm on a waterjet. It varies with machine, nozzle and material, so measure a test cut. If your machine has no compensation at all, offset the outline out and the holes in by half the kerf, for example 0.75 mm for a 1.5 mm plasma kerf. The Sketcher's Offset tool does this.

Lead-ins and lead-outs

A pierce leaves a rough crater. A lead-in starts the cut in scrap material and runs onto the profile, so the mark stays off the finished edge. Most CAM programs add lead-ins and lead-outs for you. Do not draw them into the part DXF. Place them on a straight edge or corner where a small mark does not matter. Each one adds a few millimetres of cut per pierce, so for a part with many holes enter a lead-in length in the Cut Cost Estimator for a truer time.

Minimum hole size (rule of thumb)

  • Plasma: holes under about 1 × material thickness come out tapered and rough. Use about 1.5 × thickness for clean bolt holes.
  • Laser: manages about 0.5 to 1 × thickness.
  • CNC router: an inside corner cannot be smaller than the cutter radius.

These are rough guides, not machine data. The DXF Cut Cost Estimator checks your smallest hole against them. For holes that must fit, cut them undersize and drill or ream to size. The Clearance Hole Chart gives the finished sizes.

Tabs and microjoints

Small parts can tip up into the cut path or fall through the slats. Tabs or microjoints leave a tiny bridge that holds the part in the sheet. On a router, tabs stop the part moving as the last pass breaks through. Your CAM program normally adds these, so keep the DXF outline closed.

Nesting

Before you buy material, work out how many blanks fit on a sheet. The Sheet Cut Optimizer lays out rectangular parts on a sheet and shows the yield. Use each part's overall size from the Part Maker or Sketcher size box. Your CAM nester can then pack the true shapes even tighter. When you price a job, allow for the skeleton and the gaps the nest leaves: a scrap allowance of 15 to 30% suits most nests.

Common DXF Problems and Fixes

Problem Likely cause Fix
Part opens tiny or huge Units mismatch. Millimetres read as inches is 25.4 times too big; the reverse is 25.4 times too small. Set the right units on import. Export from the tools in the units you will cut in, and check one known dimension.
"Contour not closed" or will not cut A gap between two ends, three pieces meeting at a point, or an outline split across two layers. Import the file into the DXF Sketcher. Find the red open-end markers, then redraw or snap the ends together. Keep each outline on one layer.
Jagged or slow curves Curves made of many short lines, often from a trace or a spline export. In Image to DXF, turn on Fit arcs or adjust the Simplify tolerance. Redraw key circles as true circles.
Lines cut twice Duplicate or overlapping geometry. Use Delete duplicates in the Sketcher. The Cut Cost Estimator also reports duplicates and overlaps, and how much cut length they add.
Part opens mirrored The template was scanned face down, or the software flipped the Y axis. Use the Mirror tool (I) in the Sketcher, then export again. Check any handed part, like a left-hand bracket, before cutting.
"Unsupported version" or file will not open A newer DXF version or entities the software cannot read. Save as R12. Import into the Sketcher and export again, which also drops text, splines and blocks it cannot use.

Once your CAM program has made the toolpath, you can check the code in the G-Code Viewer and Simulator before it goes to the machine.

Make Your DXF Now

Four free tools, all running in your browser.

DXF Part Maker DXF Sketcher Image to DXF Cut Cost Estimator

Frequently Asked Questions

Which DXF version should I send to a laser or plasma cutter?

R12 (AC1009) is the safest choice. It is the oldest common version, and almost every CAD, CAM and cutting program can read it. All three free DXF tools on Machinist Central write R12.

Should I add kerf to my DXF?

Usually not. Draw the finished part size and let the CAM or cutting software apply kerf compensation, outside the outline and inside the holes. Only offset the drawing yourself if your machine has no compensation, and then by half the kerf.

Why does my DXF open at the wrong size?

It is almost always units. A part drawn in millimetres but read as inches comes in 25.4 times too big, and the other way round it comes in 25.4 times too small. Check the units setting when you import, and measure one known dimension before you cut.

Can I turn a picture or logo into a DXF for cutting?

Yes. Use the Image to DXF Converter in Outline mode to trace closed shapes with their holes, then set the real size from the scan DPI, the overall width or two measured points. Traced shapes follow the pixels, so check a known dimension before cutting.

How much does laser cutting cost per part?

It depends on the cut length, the number of pierces, the material and thickness, and the shop's hourly rate. In the worked example above, a 120 × 80 mm bracket in 3 mm mild steel comes to about 2.21 each for 50 on a fibre laser at 120 per hour, but a single part hits the 50.00 minimum charge. Drop your own DXF into the free DXF Cut Cost Estimator with your rates for a full breakdown.

Are my drawings uploaded when I use these tools?

No. The DXF Part Maker, the DXF Sketcher, the Image to DXF Converter and the DXF Cut Cost Estimator all run in your browser. The geometry and the DXF file are made and read on your own device.

Summary

A good cutting DXF is simple: closed loops, no duplicates, true arcs, the right units, R12 format and a clear origin. Use the DXF Part Maker for standard parts, the DXF Sketcher for custom shapes, and the Image to DXF Converter for drawings and logos. Price the finished file with the DXF Cut Cost Estimator. Leave kerf, lead-ins and tabs to your CAM program, and always check a test cut before you run good material.