Coming to a CNC mill from a laser cutter, it is easy to get tripped up by the physical size of the bit when making designs. Any time you want to cut out an inside angle, you need to keep in mind that you can't reach all the way into an inside angle with a rounded bit. This comes up frequently when making furniture or any type of joinery; this post was inspired by the awesome examples of CNC joinery from this Make magazine post. Let's dive into the problem with inside corners and illustrate strategies to fix it.
 |
| A rounded bit prevents reaching inside corners |
The problem obviously depends on the size of your bit (let's call the bit radius R). An easy way to reduce the impact of this problem without modifying your design is to simply use a smaller bit. A laser cutter suffers from this only slightly because the 'bit size' is a tiny beam of light!
Fixing the inside corner problem
You can modify your design to compensate for this problem. There are actually several ways to cover the red area shown above.
If you have VCarve Pro, there is a tool that will do these operations automatically. Skip to the end to see how to use it.
The dog-bone
One way is to round the corner and slide it out until the entire red area is covered. It is difficult to explain with words and much clearer in diagram form!
To do this in a vector graphics program, you make a circle with the radius of your bit centered at the corner, translate it by the values in the diagram X = Y = sqrt(R^2 / 2) and do a boolean union operation with the inside corner. This method lets the part sliding into this corner just barely 'kiss' the inside of the circle, which is good for joints that take stress because the corner is still supportive. Here is what the tool path and resulting joint will look like:
The T-bone
There is another way to cover that red area, though. Instead of 'pushing' a circle into the corner of your design, you can push a circle directly in one direction, up or sideways (diagram shows up). The math for this method is simpler: you only need to push a circle up by one radius from the corner.
This method is biased in one direction, which can have a few effects:
- If your design has another piece laying on top of the joint, the circular deviation can be completely covered up.
- The corner is supported in one direction but not the other. Make sure if you want this joint to take load, plan out carefully which direction needs to be supported. If both have to be supported, you might want to use the first method
There are two ways you can fix the inside corner problem on a CNC. Few CAD programs do this automatically, but it is not hard to fix in a vector editor like Illustrator or Inkscape.
Do it automatically!
VCarve Pro has a really great built in tool for doing this automatically. From the Drawing menu, select the Create Fillets menu item (highlighted in the image below).
![]()
Do it automatically!
VCarve Pro has a really great built in tool for doing this automatically. From the Drawing menu, select the Create Fillets menu item (highlighted in the image below).
Enter your tool diameter and choose which technique you want to use.
To use the tool, simply click on an inside corner of your design. It will automatically insert the fillet in the correct position.
Warning: the fillet tool is not parametric; scaling your design after inserting fillets will scale the fillets as well. It is best to insert the fillets after the design is complete.