Fillets are one of those design features for which there seems to be no middle ground, or at least not one that is widely known. Either a part is devoid of them, and most or all edges are well-defined, or the part’s designer decided to take the opposite route, and every single edge and corner is rounded with some size of fillet radius.
Fillets can be useful in the design world, especially when parts are destined for CNC machining, which will be our primary assumption in the following examples. This article will expose the cases in which fillets are a bad idea, a good idea, and absolutely necessary (hint: corner fillets), so you can start tweaking your designs to be more cost-effective and more readily manufacturable.
Where You Don’t Need Fillets
Before talking about use cases for fillets, it’s easiest to rule out a few places where you don’t need them, because too much of something is never a good thing.
3D Printed Parts
Because 3D printing is an additive process, there’s no need to design a part assuming a tool will need to move around it and remove material, and a designer has much more freedom to utilize intricate and unusual geometries. Fillets are sometimes added for stress relief in areas of sharp geometry changes, but beyond that, there is little need for them. Pockets and internal features on printed parts can be angular or sharp-cornered, and you can even have cavities that are completely enclosed by surrounding material!
Also, keep in mind that if you’ll eventually be moving away from 3D printing towards another process, such as machining, it’s essential you start planning for the limitations of that process early on, to save time and money down the road.
Filleting the bottom edges of pockets, walls, or boss features can be used to improve aesthetics of a part or add strength to features (by reducing stress concentrations). However, fillets in these locations require the use of a ball endmill and will always make your part more expensive than square-bottomed features. This is because programming such a geometry usually requires 3D machining operations (which take longer to dial in). Also, ball endmills are by nature more fragile than their square counterparts and must machine at a much slower rate.
On a related note, filleting the bottom edge of a part will create the need for another fixturing setup, which will also increase a part’s production price.
Where Fillets Can Be Helpful
This next section will provide a few examples where fillets may come in handy, despite not being needed. Remember, however, that fillets on a CNC part add programming and machine time— and therefore cost.
Cosmetic Face Edges
When designing a part with cosmetic faces, filleting the edges of these areas can be a nice way to give your part the appearance that its faces blend seamlessly together, rather than transitioning harshly.
Adding fillets can prevent injuries from sharp edges if your parts will be handled frequently, especially if they are cut from metal. It is standard practice for machinists to hand break all sharp edges anyway, so unless you adore perfectly radiused edges, or your parts have ergonomic features with radiused areas, it might be best to refrain from doing this to save a buck or two.
Getting a dowel pin to engage with a press fit hole or a fastener to align with its female threaded mate can be tricky if the fit is tight. Usually, a small chamfer (read: bevel) is added around the edge of the hole to aid in insertion, although a fillet can also help if desired.
Where fillets are absolutely necessary
This final section explores three cases in which fillets are required in order for a part to be CNC machinable.
Internal Edges Between Vertical Walls
To cut via high-speed rotation, all CNC tooling is round and axially symmetric, so cutting a square corner between two vertical walls is literally impossible. In fact, any edge where two vertical walls meet at an angle less than 180° requires fillet addition. This is the most common piece of DFM feedback we have to give here at Fictiv about parts destined for CNC.
Internal Edges Between Angled/Organic Surfaces
Similar to the first case in this section, edges between angled or organic surfaces with less than 180° between them also need fillets. If these edges aren’t perfectly vertical, they’ll be cut with a ball endmill, and the radius of that tool is the smallest fillet size that can be left between the surfaces.
Vertical Wall + Angled/Curved/Organic Surface
In a combination of the first and second cases, you’ll need to include fillets when a vertical wall on your part meets with an angled, curved, or organic surface below it. This one can be a bit tricky to reason at first, but if you picture a square or ball endmill cutting flush along a wall, you can visualize how there will always be material remaining between the wall and the surface below, unless that surface is perfectly flat and normal to the tool.
Now that you understand the general cases for and against fillet use, there are two main standards to adhere to if you’ll be producing parts through the Fictiv platform.
Minimum Fillet Size
The smallest milling tool our vendors stock by default is a 1/32” endmill (square and ball). This is just under 0.8mm in diameter, meaning the smallest fillet it can create is 0.4mm.
Fillet Size vs. Depth of Cut
Endmills come in lengths of standard multiples of their diameter, but there’s a limit to the obtainable length, due to tool vibration and chatter past a certain ratio. Material also plays a role here—it is much easier to cut a deep pocket into a plastic or cnc aluminum than into a harder material, such as steel. What this means for fillets is that they need to be a certain size, depending on how deep a cut is needed to make the feature on which they’re included. Fictiv’s max depth of cuts are as follows:
- Steels: 5X tool diameter (10X fillet size)
- Plastics/aluminum: 10X tool diameter (20X fillet size)
Overall, we recommend sticking to 3-5X tool diameter max, to the avoid sticker shock caused by excessive machine time.
Hopefully, these pointers have helped clarify the world of fillets for you. Especially in the case of CNC machining, knowing when and when not to use these features is absolutely critical: It can save you time and back-and-forth with your manufacturer, increase part functionality, and result in a much cheaper part overall. Even in cases when you’re not currently designing for machining, it’s still a good idea to follow these guidelines, in case you ever decide to. Now that you’re equipped with the proper knowledge, share it with friends and fillet away!