How to Prepare a File for Laser Cutting in Inkscape (Step by Step)

Inkscape is free and perfectly capable of producing professional laser files. The problem is that it was not built for it: its defaults — pixels, fills, live text — are the opposite of what a machine needs.

Here is the complete workflow, in the order worth doing it.

1. Set the document to millimetres

Before drawing anything. File → Document Properties.

Change two things, not one:

• Display units to mm
• Custom size → Units to mm

These are separate fields and most people only change the first. If the document size is still in pixels, export can scale wrong even though the rulers read millimetres.

Then set the real size of your work area — say 400 × 400 mm. Working on a canvas the size of the machine bed avoids fit surprises at the end.

2. Draw with stroke and no fill

The laser follows lines. Set your objects to:

• Fill: none
• Stroke: a flat colour, thin width (0.1 mm or hairline)

Stroke width does not affect the cut — the machine follows the centreline — but a thick stroke visually hides overlap problems, so keep it thin while you work.

3. Convert everything to paths

This step is mandatory, and it is the one that breaks the most files when skipped.

• Text: select and Ctrl+Shift+C (Path → Object to Path). Skip it and the file depends on the font being installed on whatever machine opens the SVG, which it usually is not.
• Shapes (rectangles, circles, stars): convert too. Many converters handle them fine, but not all.
• Objects with path effects, blurs or markers: flatten them. Anything that is not pure geometry will not survive conversion.

Verification trick: Edit → Select All, then read the status bar at the bottom. It should say only "path". If it mentions "text" or "rectangle", there is work left.

4. Find open paths

A cut outline has to be closed. One microscopic gap and the part will not release from the sheet.

To find them: node tool (N), select the object and press Ctrl+A to select all its nodes. The status bar reports how many nodes are selected. A closed path has no loose ends; on an open one, the end nodes render as squares that look different from the rest.

To close them: select the two end nodes and press Ctrl+J (join nodes), or use the join-with-segment button.

On files traced from images this can appear dozens of times. If that is your situation, it is usually cheaper to redo the trace with better settings than to close gaps by hand.

5. Remove duplicate paths

This is the most expensive mistake: the machine cuts the same outline twice, takes twice as long and scorches the edge. And it is invisible on screen, because one line sits exactly on top of the other.

How to deal with it:

• Select all and press Ctrl+Shift+G several times to fully ungroup.
• With everything selected, Path → Union (Ctrl++) merges overlapping shapes and eliminates coincident lines. Careful: this also merges shapes you wanted kept separate, so apply it to logical groups rather than blindly across the whole document.
• For parts that deliberately share an edge, position them so they share exactly the same line and join them. You cut once instead of twice: less time and less heat concentrated at that joint.

Another route is opening the XML editor (Ctrl+Shift+X) and checking for two path elements with identical d attributes.

6. Assign colours per operation

The industry convention, recognised by LightBurn and most software:

• Red (#FF0000) — cut
• Blue (#0000FF) — score or mark
• Black (#000000) — engrave

Use pure, flat colours. A slightly different red is read as another layer and you end up with more operations than you intended.

With this in place, you assign different power and speed to each colour in the machine software without touching the file again.

7. Verify real dimensions

Before exporting. Select a part and read the W and H fields in the top toolbar, with units set to mm.

If you designed something that should be 100 mm and it reads 133.33 mm, you have the classic 96-versus-72 DPI mismatch. Scaling by 0.75 corrects it, but it is better to fix document properties and re-export, because manual scaling accumulates rounding errors.

Where there are joints — tabs, slots, boxes — measure the actual gap too. Remember the laser removes its own kerf width, so a slot comes out slightly wider than drawn.

8. Save and export

Save as Plain SVG (File → Save As → Plain SVG), not Inkscape SVG. Inkscape SVG carries its own metadata that some converters do not digest well.

From here you have two routes:

• Import the SVG into LightBurn or similar. This is the usual and easiest path: the machine software handles G-code generation.
• Export G-code from Inkscape itself, using an extension such as the J Tech Photonics Laser Tool. Free, but more manual setup.

The trade-offs between the two are covered in the SVG to G-code guide.

Final checklist

Before sending anything to the machine:

• Document in mm, both size and units
• Everything converted to path — no live text
• No fills, strokes only
• Cut paths closed
• No stacked duplicates
• Pure colours separated by operation
• Real dimensions verified in mm
• Saved as Plain SVG

When you are starting from an image

All of the above assumes you draw the vector yourself. If what you have is a PNG or a photo, there is a tracing step first — and that is where most of the open and duplicate paths from steps 4 and 5 come from. Inkscape's Trace Bitmap works, but it needs a lot of cleanup afterwards.

MEZ Laser handles that step and returns closed, non-duplicated paths, letting you skip the most tedious part of the workflow.