Inkscape is a free vector graphics editor for all major platforms, generally it is aimed at art and design users but it does have an option for generating G-Code for use in your favourite CNC software. While Inkscape doesn’t have many of the functions of proper CAD/CAM software it is an relatively easy place to start for creating basic designs, I have been using it to make boxes out of 3.5mm plywood.
These notes are based around my cheap CNC machine sold as an CNC3018 by a variety of Chinese manufacturers on Amazon and eBay, the included controller is a Woodpecker CNC board (Ardunio clone) I have upgraded to GRBL v1.1 and I am using version 0.92.4 (April 2019) of Inkscape with the included Gcodetools.
This post focuses on setting up Inkscape for the CNC machine and producing the g-code from your drawing, it is not intended to be an Inkscape tutorial.
With a new drawing set your Document Size, this should be the same as your CNC bed, in my case this is 300 x 180mm. From the Inkscape menu go to File > Properties and in the Page Tab set the Display Units (millimeters in my case), the Orientation to Landscape and Page Size width: 300 and height: 180. In the Grids Tab set the Grid Units to mm and the Spacing X and Spacing Y to 1.0. Back on your main page, turn the page grid on with: View > Page Grid.
By default Inkscape scales the stroke/line width when you resize a shape, to prevent this click the the fourth box from the right in the top icon bar “when scaling objects, scale the stroke width by the same proportion”
You can save this as a template, such as: CNC3018.svg or as the document default with: default.svg by saving the file to your templates directory:
On Linux and OS X: ~/.config/inkscape/templates/
On Windows: C:\Users\<username>\AppData\Roaming\inkscape\templates
The lines you draw will need to be the same width as the bit you are using in the CNC machine. Draw a rectangle, Right mouse click on the rectangle and select Fill and Stroke…. In the Fill Tab click the X – no paint box and on the Stroke Style tab set the width to that of the bit you are using – 1.5mm, subsequent rectangles will be in the same style, other shapes will need to be setup this way too. The colour of your lines should be black, there is some functionality for different colours to represent different depths but I have not yet worked out how to do this.
Layout Tips for G-Code Routing
Remember to check the dimensions of the cuts, with an outside cut such as the width and height of a box side you need to measure for the inside of your rectangle, for holes in your box measure to the outside edge, Inkscape sets distances to the outside edge.
For positioning holes for switches and the like, I add thin lines 0.1mm thick as guides and make use of the width/height settings as well as the Object > Align and Distribute options. A pair of digital vernier calipers are a great aid to discovering the required sizes. Remember to delete these before G-Code encoding.
When generating the G-Code each shape will be seen as an individual object, so lets say you want to have two sides of your box cut from a single sheet of plywood, this would be two rectangles abutting each other with a side to be cut overlapping. As it takes four passes to cut each shape 1mm at a time, this means it’ll take six passes down the centre. To fix this select both rectangles and then Path > Combine followed by Path > Difference to make a single object.
Outputting to G-Code
Now that you have completed your drawing, save your work then convert your objects to paths by selecting all objects then Path > Object to Path. You may also want to place your drawing near the bottom left of the document, as this is where the CNC router starts. Now using Gcodetools there are three things you need to do to produce the G-Code file. None of the Gcodetools windows close automatically when apply is clicked, you will need to do that yourself. From the Inkscape menu:
1. Extensions > Gcodetools > Tools Libary…
Select Tools Type: cylinder and click apply In the overlarge green box that appears you will need to set the tool diameter and feed speed.
This can be a bit fiddly as the text can become detached from the box and the settings lost, what seems to work most reliably for me is to change to Text Objects (F8) click on the numbers you want to change and once done go back to Select and Transform (F1). Resize the box afterwards to check that it is still working – if the green box moves but the text does not then Ctrl-Z a few times and try again.
|Diameter||10||1.5||tool bit diameter in mm|
|Feed||400||300||speed while cutting through the material in mm/second|
|Penetration feed||100||100||Plunge speed in the material in mm/second|
|Depth Step||1||1||Depth of cut on each pass in mm|
2. Extensions > Gcodetools > Orientation Points
This tells the g-code where to start, normally bottom-left on the CNC Set the following:
– Orientation type: 2-points mode
– Z Surface: 0mm – this is the top of your surface
– Z Depth: -3.4mm – this is the thickness of material to cut, a negative number
3. Extensions > Gcodetools > Path to Gcode
This creates the G-code file, in the Preferences Tab set the following:
– File: output filename
– Directory: output directory
– Z safe height: 5mm – height above the work surface when moving between cuts
The filename once set doesn’t change, an incremental number is appended to the output filename. Click the Path to Gcode Tab before clicking apply (this appears to be a bug).
Your image will be updated to show the g-code routing, give this a visual check to ensure that all objects have been coded and that it looks right, the path to be taken should be in colour and contain arrows showing the direction of the router.
If there are too many arrows or if a line has arrows pointing in different directions then there may be an object underneath, check on your original artwork, in the image with the three circles below you see that A has not been converted to a path with Path > Object to Path, B has a duplicate object underneath and C is correct.
The generated G-Code does not appear to include the Spindle Motor Start command – So remember to start the spindle manually in your CNC software before running the G-Code – its interesting how easily these bits break with a sideways load. Remember if you are cutting trough rather than engraving, don’t forget to put a layer to sacrifice between whatever you are making and the CNC’s bed, I use 5mm MDF/Fibreboard.