You’ll often encounter inside corners when designing parts for milling. Two common situations in which this may occur are while designing parts that mate together and when adding a slot for something to move along. Ensuring your parts can fit together can be way more complicated than you’d think. Of course, the easiest solution is to avoid inside corners altogether, but for the sake of this article, let's assume that is not an option for your design.
Rounded inside corners are a consequence of the way milling tools cut due to their geometry - they are round, so the inside corners they create are therefore also round. Notice in the images below how the tool is not able to access the entire corner of the pocket:
So, how do you get around this? The best way to combat this is to design your parts in a way that is compatible with the process. For example, when designing two parts that mate together, radius the edges of both:
The manufacturability of the corners will depend heavily on the size of the corners, and their location. Even if all corners have a radius, a small tool may not have enough cutting length to reach the bottom of a pocket, as smaller-radii tools are shorter than large tools.
Consider the below example of two pockets with the same size but different corner radii:
The small tool, despite being the correct size to cut the corner, does not have enough cutting length to reach the bottom of the pocket. The larger tool is both large enough to cut the radius and long enough to reach the bottom of the pocket. It can also be moved faster in the milling machine and remove more material per pass.
A good rule of thumb when considering corner radii is to set it at least ⅙ the depth of the pocket. For example, at Plethora, the smallest radius supported is 0.032”, which indicates that the maximum depth of a feature with corners of this radius is roughly 0.138”.
Consider another example: milling a u-shaped piece. In this case, the width and depth of the inside cutout will drastically affect manufacturability. A wide slot can be accessed by a large tool and milled, although a thin slot requires a smaller tool that may not be able to reach the bottom of a deep pocket:
Also consider the implications of adding an internal corner at the bottom of the deep pocket. Square corners force the part to be oriented with the slot vertically, in order to mill the bottom flat, but when an internal corner is applied, the part can be flipped on its side and the slot can be cleared without issue:
The radii of the rounded corners in your design isn’t the only thing worth considering. As touched on in the last example, the angle at which the tool approaches the work is critical as well. Clever workholding allow all sides of a part to be milled, one after another, so even if there aren’t rounded corners, some features can still be machined without issue.
Consider the following examples. Despite their hard edges, these are both still manufacturable, thanks to the fact that the slots run through the entire piece, allowing the tool to clear through it:
However, the below example is not manufacturable, as the slot does not run all the way through the work, and the tool needs to clear a corner:
This can be fixed by rounding the two corners in the bottom of the pocket:
It can also be fixed by rounding the two vertical edges, making room for a large tool to cut in from above:
For situations where rotating a workpiece to change the approach angle of the tool isn’t possible, such as during the milling of large sheets of material on a router, a couple types of corner reliefs can be used.
If you find yourself in a situation where the internal pocket needs to accept a mating part that has square edges, adding t-bones to the corners is a nice solution, and is straightforward to add to your model in CAD.
Another way to add internal corners to your model is the nicest looking, but also the most complex to add into your model - dog-bones!
The symmetry of dog-bones is more pleasing to the eye than t-bones, and provides symmetric support to the corners of your square mating part.
Thankfully though, there are a multitude of ways to deal with internal corners in milling applications, so it's recommended that you choose the solution that works for you. When it comes to considering the feasibility of your design, though, the best solution is to imagine how a cutting tool will access all of the features of your part. And remember, the Plethora add-in provides real-time DFM feedback while you design, including when you need to add internal corners or reconsider tool accessibility.