How to Prepare a DXF, DWG or STEP File for Contract Cutting: A Technical Guide

A waterjet or laser cutting machine turns your vector file directly into a toolpath. In other words, the machine reads exactly where your lines start and end, not what you meant to draw. A double-drawn edge, an open contour, or a file saved in the wrong unit can turn into hours of back-and-forth before production even begins, or worse, a scrapped part. A clean DXF, DWG or STEP file speeds up your quote and helps ensure your tolerances are actually met.

In practice, most of the files we receive share the same small but recurring problems: ambiguous units, leftover layers, scale errors, and raster (pixel) images mistaken for vectors. In this guide we walk through the checklist our team runs on every file before it reaches the machine, so you can get an accurate price and the shortest lead time on the very first quote.

For 2D flat sheet or plate cutting, DXF is the safest format because virtually every CAM package reads it cleanly. DWG works too, but version compatibility can occasionally cause problems, so we recommend exporting to a broadly compatible version such as R2010. PDF is useful for visual reference only; because the lines inside a PDF are often scaled or rasterised, it is not reliable as a production file. If you do send a PDF, always attach a genuine vector DXF alongside it.

If the part has true 3D geometry (bends, steps, taper angles, 5-axis waterjet), send a STEP file (.stp / .step). Because STEP carries genuine solid geometry, no dimensions are lost, and our team can derive 2D section profiles straight from it when needed. In short: DXF for flat cutting, STEP for volumetric and 3D work, with DWG and PDF treated as complementary rather than primary files.

A cutting machine interprets a part through a closed contour (a closed polyline): material on the inside, empty space on the outside. If the start and end points of a line do not meet exactly, the contour stays open and the machine either skips that profile or cannot tell where to pierce. A 0.01 mm gap is invisible to the eye, but CAM software catches it every time. That is why every outer edge and every hole must be a single, closed polyline.

To verify this, select the geometry in your CAD program, run the join command, then query the area: a closed contour returns a calculable area, an open one does not. Using a single closed polyline instead of many separate line and arc segments both simplifies the file and prevents unnecessary stops during cutting. Make sure inner holes are also closed on their own and kept separate from the outer contour.

The standard unit in manufacturing is the millimetre. The DXF format itself does not always carry unit information reliably, so drawing at 1:1 scale in mm is critical. Drawing in inches but assuming millimetres scales the part by a factor of 25.4, and if this slips past the quoting stage, the wrong material gets cut. The safest approach is to add a known reference dimension (for example a 100 mm edge) or to clearly state the overall outer dimensions in your quote notes.

To confirm the scale, open the file and measure a known edge: if you drew 100 mm, you should read 100 mm on screen. Drawings pulled from a PDF can hide a 'fit to page' reduction, so never rely on a PDF alone as your dimensional source. Once the unit is unambiguous, the price for waterjet and laser cutting is also calculated correctly, based on the true material area.

Design files often contain dimension lines, hatches, text, centrelines, and reference layers. To the machine, all of this is noise that gets confused with the geometry to be cut. The production file should contain only the cutting contours; dimensions, text, and helper layers should be deleted or clearly placed on a separate informational layer. Where possible, consolidate the cutting geometry onto a single layer.

The most insidious problem is duplicate lines, where the same edge is drawn twice on top of itself. In laser cutting this means the same path is cut twice (edge burning, wasted time and gas), and in waterjet it causes overlapping paths. Run the overkill or duplicate-cleanup command in your CAD program to remove overlapping and coincident lines. Our team repeats this check on arrival, but a file that comes in clean at the source shortens lead time and removes any risk of misinterpretation.

Every cutting method has a physical limit. As a practical rule, a hole becomes harder to cut as its diameter approaches the material thickness; in thick material especially, holes smaller than the thickness may not be cut reliably. In abrasive waterjet the kerf is typically around 0.8-1.5 mm, and sharp inner corners are rounded off by roughly that radius. With fibre laser, very sharp details are possible in thin sheet, but minimum hole diameters and bridge widths grow as thickness increases.

So if your drawing contains very thin transitions, hair-thin bridges, or holes that are disproportionately small for the thickness, it is best to flag these in your production notes. For precision work where micro-detail must be preserved, we evaluate material, thickness, and method together and recommend the most suitable technology. When tolerance is critical, write the allowable tolerance range next to the nominal dimension so the machine can apply the correct offset.

A vector defines geometry with mathematical lines and curves; it never degrades however much you scale it, and the machine knows exactly what to cut (DXF, DWG, STEP, AI, EPS). A raster is an image made of pixels (JPG, PNG, BMP) and cannot be used directly by a cutting machine, because where each pixel ends is ambiguous. Sending a JPG of a logo 'instead of a DXF' is not the same as sending a production-ready file.

If all you have is a photo or a scanned image, it must be converted into clean contours through vectorisation (tracing). A high-resolution image with sharp contrast and crisp edges makes this far easier; with blurry or low-resolution images, edges have to be guessed and need manual correction. As long as you supply a reference dimension, our team can help you turn a photo or hand sketch into a cut-ready vector file. Even so, the most accurate result always comes from starting with a vector drawing where possible.

While file cleanliness is enough for standard contract cutting, in high-precision work such as aerospace and defence the file itself becomes part of a documented process. For these jobs, each part should carry a revision number, material specification, critical dimensions, and a tolerance table defined together with the drawing. We run our processes with aerospace-grade discipline, in a way that supports measurement and material traceability; depending on the request, delivery with a material certificate and an inspection report is possible.

A practical tip: clearly mark critical tolerances on the drawing, separate functional (assembly-critical) dimensions from free ones, and include the revision in the file name (for example part_v3.dxf). This discipline removes the risk of producing from the wrong version and speeds up the inspection and approval cycle on high-precision jobs.