CNC Routing

There are a few basic principles to follow to ensure the parts you receive are as you’ve designed on your computer.

There are numerous CAD programs out there that all serve the same purpose but operate in different ways. The analogy can be like foreign languages and regional dialects. For humans we can politely smile and gesticulate, unfortunately computers can’t.

Incorrectly cut parts caused by these communication errors cost time and money. Thankfully many of these issues can be avoided by having a basic understanding and following some simple rules.


The language of machining is vectors. Vector artwork is the most basic of computer drawing, the fundamentals are;

  • Lines: point A to point B.
  • Circles: a 360 degree line a set distance around a single point.

All vector drawings are made with variations and combinations of these two principles.

a to b

In basic terms, the CNC router can only see vectors. When we program the machine to cut we stipulate one of the following conditions:

  • Cut on the vector
  • Cut to the left of the vector
  • Cut to the right of the vector.

And for closed vectors like circles, squares, rectangles etc:

  • Cut inside the vector
  • Cut outside the vector

In most cases, your artwork should contain only closed vectors. Problems arise when your vectors are open, points are not snapped together or vectors are overlapping. Most programs have a “Join”, “Close” or “Combine” functions.

On left right
inside outside

Notes for Illustrator and Sketchup users. 

It is important to make the distinction between engineering software and graphics software. Engineering software creates accurate and defined measurements; graphics software creates approximate information for visual display.

For example, Sketchup will generalise a render to make it appear complete on the screen which can cause problems when you ask a machine to follow a vector.

Illustrator is guilty of generating multiple lines. When constructing a drawing, ensure your line thickness is set to hairline and is a single stroke. 

Cutting methods

There are 4 main processes of CNC routing:

  • Profiling – The router cuts on the left or right side of the line and through the entire thickness of the material.
  • Pocketing – The router cuts / removes all material within a vector, the depth of cut can also be defined.
  • Engraving – The router cuts along the vector line, useful for slotting or labelling parts.
  • V-carving – The router cuts within a text vector, this is used for signage text.
  • 3 axis surface modelling – This is for carving detailed 3D objects out of foam and other thicker materials.


Within the document, please include the following text notes:

  • Material: WBP, Birch Ply, ABS…….
  • Thickness: 9mm, 12mm, 18mm……..
  • Number of parts: x20
  • Pocket depths 

Colour coding

Please colour code your 2d files as follows:

  • Profile cut = Black
  • Pocketing = Blue
  • Engraving = Red
  • V-carving = Green


The file you are creating should be scaled 1:1 and in millimetres. It is good practice to drop in a reference square of a labelled size to avoid those “Stonehenge” moments.

File type

We only accept .AI .DWG .DXF or .3DM (rhino). These are the .jpeg of the CNC world, Rhino can read them fluently and most other software packages are able to export them.


If you are cutting multiples of the same part, we only need one drawing to work from. Please don’t send a drawing with x500 of the same part – we will copy and arrange the parts on a sheet in the most suitable and efficient way for cutting.

Do not send the whole file, just the part you need cutting!

File size

Vector artwork should be small. Chances are if your 2D artwork is over 3MB there may be something wrong with the file. Go back and check that you are not also exporting any unnecessary parts or layers of your drawing.


Understanding tolerances is very important for successful fabrication design. Problems originate from the perfect and binary world of computers, whilst what you see on screen is 10mm there a number of contributing real-world factors that can affect measurements of finished parts.

  • Software –  It is a little known secret… machines can’t actually cut circles. The code that drives the router breaks a circle vector down into a series of tiny straight lines, point A – B, point B – C, etc. The tolerance we work to is 0.03mm, this means the cutter does not deviate further than 0.03mm from the drawn vector. Although small, this tolerance must be considered for small radiuses and where parts are interfacing or joining.
  • Machine deflection – No machinery is 100% precise. Machinery with multiple moving parts has tolerances in it that allow it to move and flex within the gantry materials. When servicing our router we check this deflection – at present the deflection is 0.05mm on X and Y axis with 0.09mm on the Z axis. To put that in context standard printer paper is 0.12mm
  • Cutter deflection – As a cutter is ploughed into a material it will bend slightly, this is more noticeable on cutters with a diameter smaller than 5mm. When travelling along a straight vector the deflection remains fairly constant, when making hard directional changes such as corners ≥90 degrees it can be visible on thicker materials. As designers, you can reduce this effect by adding a radius to your corners. As machinists, we prefer to use 6mm cutters for general purpose machining as the deflection is less. For parts that require cutting with smaller diameter cutters, we can compensate by reducing the feed rate in these areas.
  • Cutter wear –  We use premium quality Belin solid carbide cutters.  These tiny bits of metal are an absolute marvel of engineering. Carbide is one of the hardest wearing materials available and when combined with precise geometry the cutter edge is razor sharp for many machining hours. Spinning at +18,000 rpm means the cutting edge is making 300 slices a second, so give it some credit. Inevitably towards the end of a cutter’s harsh and brutal existence, the edge becomes less pointed and more rounded with a minor reduction in cutter diameter. Rather than cutting, the material is pulled apart, leaving a scratty edge. Be assured, as machine operators and owners we step in way before this occurs to ensure you get a quality cut and we don’t put any unnecessary wear on the spindle and running gear.
  • Materials – Stock thicknesses vary wildly. For example, 18mm ply can fluctuate between 17.3mm – 18.4mm. For thickness critical parts please request or measure your stock with a vernier calliper and apply to your design. Cast acrylic can be up to a 1mm thinner in the center of a sheet due to the nature of its manufacture, please take this into account when designing your parts. Always measure, and remember to remove the protective film when you do!
  • Thermal expansion – As temperature increases, all materials increase in size. The size increase is proportional to the density of the material. For example, acrylic will expand more than ply. The larger the piece the more pronounced with effect will be. Its something to consider when rigidly joining two different materials, if the expanding part has nowhere to go it will bow anyway it can or rip itself from an adhesive. Acrylic has one of the highest thermal expansion rates, a temperature difference of 20 degrees on 1 meter can increase length by 1.5mm! We have to make these considerations when transferring set pieces and props from a cold workshop to the extremes of high powered studio lighting.