The part in question, with tooling, rendered in Fusion 360.
People often contact us asking if a specific part they've designed can be made with a desktop CNC. In this article, we use one example part to show you how to determine if a part can be milled and what size tools and raw material we’d need.
In this example, community member Larry sent us his design for an adapter to relocate the brake fluid reservoir on his kit car. The reservoir currently connects directly to the master cylinder and feeds it with fluid, but it's very hard to check the fluid level or add more due to its location in the car.
Stock Master Cylinder and Reservoir
Master Cylinder Reservoir Adapter Design
This adapter will connect to the master cylinder in place of the reservoir and provide a connection for hoses that will be plumbed to a remote reservoir located in a more accessible area. Larry is interested in milling this part because he found a version he 3D-printed to be too weak.
Larry's 3D-Printed Prototype
By knowing the background of the part's function and taking a look at Larry’s design, we can determine functional requirements for the part that will influence the milling strategy. For this part, to avoid leaks, achieving a tight seal with the master cylinder and hose fittings is critical, so we we'll need tight tolerances and good surface finish on select surfaces. The part will also have to be resistant to brake fluid, as well as to the heat and vibration inside the car’s engine compartment, which limits the material choice to acetal resin or aluminum.
Feature Geometry and Setups
The first thing we usually look at is the type of features on the part. An end mill can cut holes, slots, pockets, and profiles but can’t create overhangs or complex internal cavities. For example, the deep rectangular pocket in the middle of this part is straightforward to mill, but if it were wider at the bottom than the top, an end mill would not cut it.
Features, clockwise from top-left: Clearance pocket, gasket grooves, fluid interface bosses, through holes, pipe thread bores, top contour, part outline, retention pin hole.
On this part, most of the features will be accessible from the top with a normal flat end mill, with two exceptions: the retention pin hole must be cut from the side, and the pipe thread bores must be cut from the bottom.
Feature Size & Tool Selection
After evaluating the part geometry, we look at the dimensions of the features to look for further limitations. Features that are very deep relative to their width can be difficult or impossible to mill. Large-diameter end mills are strong and can mill into deep cavities, while smaller diameter end mills are limited to shallower cuts.
We start by seeing which features can be milled with a ⅛”-diameter flat end mill and then determine if smaller end mills are necessary to complete the part. On Larry’s part, the smallest features are the through holes and gasket grooves, and a ⅛” flat end mill can fit in both, so we won’t need a smaller tool.
Checking 1/8" end mill clearance in small features.
After seeing what diameter tool is needed, it's important to check for deep areas that will be hard to reach. If the tool doesn't stick out far enough from the collet, the collet and nut will collide with the part. The pocket in the middle is 0.862” deep, so we need at least this much exposed tool length, or "stick-out," to mill this feature.
If we want to mill the part outline from one side, we’ll need more than 1.1” (the overall height of the part) of stick-out. Milling part of the outline from the top and the rest from the bottom is possible, but achieving perfect alignment between the two operations would be difficult, so we'll choose a tool that can do it in one.
Checking stick-out length.
When placing the tool in the collet to install it in the spindle, we have some freedom as to how much the tool sticks out, but it's best to have the collet at least fully engaged with the shank. We're using an ER-11 collet that is 0.7” tall and a bit fan that is 0.185” tall, so we need a tool that's at least 1.985” long for the part outline. A common length is 1.5”, but we found a 2.25” long end mill to achieve the reach we want.
The flat end mill will work well for the through holes, fluid interfaces, and clearance pocket. With the right strategy, it will also mill the contoured top surface with good results. After milling all of these features, we'll use a chamfer tool to break the sharp edges and give the part a professional finished look.
We’ve determined that we can mill the part and chosen the tools to do it, so now we must make sure the part and the stock we'll mill it out of will fit inside the CNC machine. In this case, the CNC machine is the Othermill Pro. The part itself is 3.9” long and 1.1” deep and tall. In most cases, starting with stock that's slightly larger than the part in all three dimensions is desirable, so we selected 1.25” square bar stock cut to 4” long. The Othermill Pro has a working volume of 5.5" × 4.5" × 1.35", so the stock will fit and leave some extra room for fixturing.
Alignment and Fixturing for Multiple Setups
Now that we’ve found workable options for cutting tools and stock, we need to make sure that we won’t run into any issues making this part in three separate setups. For each setup, consider how to hold the part securely and how to accurately position the features you want to mill.
When switching from one operation to another, some misalignment is possible. By cutting most features in one setup from the top, we can ensure the best positional accuracy between these features. For example, to fit well, both fluid interfaces must line up with the mating features on the master cylinder. The distance between them is critical, but since both interfaces can be milled in one setup, achieving a good fit is possible.
On the other hand, the location of the pipe thread bores on the bottom of the part is not as critical. They'll work as long as the fluid can pass from the through hole into the bore, so milling these features in separate setups shouldn't be a problem.
To minimize the possibility of misalignment from one setup to the next, we start by milling as many features as possible in the first setup. We'll mill everything that is accessible from the top and complete the part outline. To allow access to mill the outline, we need to hold the part using the bottom surface only, which can be done using Nitto double-sided tape. We’ll leave some extra stock under the part and remove it in the next operation.
1st Setup: Top
In the second operation, we flip the part upside down. The top surface, now facing down, doesn't offer enough surface area for double-sided tape to be effective, so we remove the spoilboard and use the Precision Fixturing and Toe Clamp Set. We locate the part by aligning one of the completed sides against the tall alignment bracket and clamp it in place with a toe clamp on the other side. In this setup, we remove the extra stock from the first operation, face the bottom surface of the part, and mill the pipe thread bores.
2nd Setup: Bottom
Finally, we place the part on its side, aligning the bottom surface to the tall alignment bracket and securing it with a toe clamp on the top surface. This provides adequate fixturing and alignment to mill the retention pin hole.
3rd Setup: Side
Now that we’ve determined whether or not we can mill this part, decided which tools to use, and come up with a fixturing and alignment strategy for each setup, it’s time to move on to CAM.
In the next article, we’ll explore what types of toolpaths we can use to machine this part, how to set up each operation in Fusion 360, and show you the details to look out for when generating G-code for the Othermill Pro.
In the meantime, if you have a file that you'd like us to take a look at and see if it can be milled, submit a file cut request below.