Here we will explain the basic principles to follow to ensure the parts you receive are exactly as you are expecting.
There are numerous CAD programs out there that all serve the same purpose but operate in very different ways. Just like with foreign languages and regional dialects, the various programs communicate the same message but with different ‘words’. For humans, we have the option to politely smile and gesticulate to help get our message across but unfortunately computers don’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 of the routing process and following the simple rules set out below.
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.
In basic terms, the CNC router can only see vectors. When we program the machine to cut we stipulate one of the following conditions:
- Make the 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. To avoid these issues, most programs have a “Join”, “Close” or “Combine” functions.
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 whereas 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 often guilty of generating multiple lines which will then tell the machine to make multiple cuts. Therefore, when constructing a drawing, you should ensure your line thickness is set to hairline and is a single stroke set to 100% opacity.
There are five 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 and removes all material within a vector. The depth of cut can also be defined.
- Engraving – The router cuts along the vector line, which is useful for slotting or labelling parts.
- V-carving – The router cuts within a text vector. This is used for signage text, for example.
- 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 required: WBP, Birch Ply, ABS…
- Thickness of material: 9mm, 12mm, 18mm…
- Number of parts: x20
- Pocket depths
Please colour code your 2D files as follows so we make the correct cut:
- Profile cut = Black
- Pocketing = Blue
- Engraving = Red
- V-carving = Green
We only accept .AI .DWG .DXF or .3DM (rhino) as these are the .jpeg of the CNC world. Rhino can read them fluently and most other software packages are also 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!
Vector artwork should be small, so 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 because problems can originate when you try to recreate a perfect, binary computer design in the physical world. Whilst what you see on screen is precisely 10mm, there are a number of real-world factors that can affect the actual measurements of finished parts.
- Software – It is a little known secret that machines can’t actually cut circles. The code that drives the router bit, 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 should be considered for small radiuses and where parts are interfacing or joining.
- Machine deflection – No machinery is 100% precise as machinery with multiple moving parts has tolerances built within it that allow it to move and flex. When servicing our router we check this deflection and at present the deflection is 0.05mm on X & Y axis, with 0.09mm on the Z axis. To put that into context standard printer paper is 0.12mm thick.
- Cutter deflection – As the cutting bit is ploughed into a material it will bend ever so slightly. This is more noticeable on cutters with a diameter smaller than 5mm. When travelling along a straight vector the deflection remains fairly negligable. However, it can be visible on thicker materials when making hard directional changes, such as angles ≥90 degrees. As designers, you can reduce this effect by adding a radius to your corners where possible. As machinists, we prefer to use 6mm cutters for general purpose machining as the deflection is less. If you have parts that require the use of smaller diameter cutters, we can compensate by reducing the feed rate (cutting speed) in these areas.
- Cutter wear – We always 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 precision geometry, the cutter edge stays razor sharp for many machining hours. Spinning at +18,000 rpm, the cutting edge makes around 300 slices a second, so give it some credit! Towards the end of a cutter’s harsh and brutal existence, the edge inevitably becomes less pointed and more rounded and there is a minor reduction in cutter diameter. Rather than creating a clean cut, the material is pulled apart leaving a scratty edge. Rest assured, as machine operators and owners we step in way before this occurs to ensure you get a high 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 measure your stock with a vernier calliper and apply the measurements to your design. We can also double check measurements of our stock materials by request. Cast acrylic can be up to a 1mm thinner in the center of a sheet due to the nature of its manufacture so please take this into account when designing your parts. Always measure first, and remember to remove the protective film when you do!
- Thermal expansion – As temperature increases, all materials increase in size. This 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 the effect will be. It is something to consider when rigidly joining two different materials. If the expanding part has nowhere to go it can bow away or rip itself from an adhesive. Acrylic has one of the highest thermal expansion rates and a temperature difference of 20 degrees on 1 meter can increase length by 1.5mm! It is important to make these considerations, for example when transferring set pieces and props from a cold workshop to the extremes of high powered studio lighting.