CNC machining is one of the most widely used prototyping and manufacturing methods today, especially for metal parts. Even if a part is cast, there is a good chance that some sort of machining will also be necessary to finish it. Countless hardware developers and engineers have benefited from the automation of CNC machines to “hog out” their product from a hunk of metal.
Most of the details such as tooling, spindle speed, cutter type, and depth of cut, are taken care of at the machine shop, but there are some things you can do while designing your product to not only make sure it can be made, but also to create a lean product that doesn’t break the bank. We’ve gathered some best practices for you to keep in mind while designing your product, separated into 3 sections: drilling, milling, and turning.
Drilling refers to the operation of creating holes in a piece of material. Drilling tools are designed for vertical cutting and have a conical tip, allowing them to plunge deep into a material.
Through Holes vs Blind Holes
A through hole goes through the entire part, whereas a blind hole does not. Thru holes have the benefit of being easier to clean out, but are sometimes conflicting to requirements, for instance on the external shell of a vacuum-sealed chamber.
Avoid Flat Bottom Holes
Flat bottom holes should be avoided. Blind holes are cut with drilling tools, which have conical tips. Flat bottom holes must be cut with an endmill, which are not designed for drilling operations.
Keep Hole Depth to < 5x Diameter
The depth of your hole should not be more than 5 times the diameter of the hole, because tip wander can occur with long holes. For instance, a .25” hole should be no deeper than 1.25”.
Avoid Partial Holes
Partial holes should be avoided because there is a high chance of tip wander, especially when the drill axis is close to the edge of the material.
Keep Drill Axis Perpendicular to the Surface
The drill axis should be perpendicular to the surface so that tip wander does not occur. In a lot of cases, a shallow, flat bottomed pocket can be milled onto the surface of a round part so that the drill enters perpendicular to the surface.
Use Standard Drill Sizes
Use standard drill sizes. This can be applied to all cutting operations: designing your part to be cut by standard, common tools will save you lots of money! Machine shops can create new tools of unusual size, but this is a costly process and chances are you can tolerate a standard .125” hole instead of a .123” one.
Print out a chart like this and keep it handy.
Threaded holes should have between 1-1.5D thread engagement. For instance, a ¼-20 machine screw should have a thread engagement between .25” and .375”. Depending on the application of your product, you may want even more thread engagement, but 1.5D is comfy.
While we don’t require drawings for standard CNC machining, any threads should be called out with a drawing, uploaded to Fictiv as a PDF, as that information rarely makes it into the solid model.
Avoid Deep Taps
Deep taps should be avoided because long tools have a tendency to vibrate and wander, resulting in a flawed tap.
Milling refers to the machining process of quickly subtracting material from raw stock until the desired shape is achieved. Milling is performed by round cutters (most commonly endmills) which chip away material laterally with shallow depths of cut.
Avoid Sharp Internal Corners
Because milling is done with round tools, sharp internal corners cannot be achieved. Radiused corners are required, and must be larger than the cutter to be used. For instance, a ¼ ” cutter can be used for fillets larger than ⅛ ”.
Avoid Deep, Narrow Slots
The final depth of cut of an endmill should be not greater than 15 times the diameter for plastics 10 times the diameter for aluminum, and 5 times the diameter for steel. This is because long tools tend to deflect and vibrate, resulting in bad surface finishes. For example, a slot for a machined steel part that is .55” wide (which will be cut using a .5” endmill) should be no deeper than 2.75”. Internal fillet radius, the above point, is also dependent on this, meaning that any internal radii for this example should be greater than .25”.
Design with Largest Possible Internal Radii
The larger the cutter, the more material can be removed at one time, meaning less machining time and less cost. Always design with the largest allowable internal radii. Avoid radii less than 0.8mm whenever possible.
Pro Tip: Make your fillets slightly larger than the radius of the endmill, for example, a radius of .130” (3.3mm) instead of .125” (3.175mm). This will produce a smoother path for the mill to take, resulting in a nicer finish.
Turning refers to parts created on a lathe, generally with circular symmetry.
Avoid Sharp Corners
Avoid sharp corners, both internal and external. Internal corners should be radiused so that the tool doesn’t run up to a large surface. Think about smooth tool paths.
Avoid Long, Thin Parts
Avoid long, thin turned parts as there is more of a chance of them spinning unstably, causing them to chatter against the tool. If a long part must be made, try to accommodate a center drill on the free end and use a center to keep the part spinning straight.
In general, any feature that is added to a turned part should be symmetric about the turn axis.
If you’ve got a good understanding of the above practices, check out these tips to really solidify your lean design. The first few tips are about increasing the speed of machining and minimizing the start-to-finish fabrication time, thereby reducing cost.
Create Easy Setups
Create easy setups for your machine shop. Think about how your part will be held during the machining process. The easiest setup is a vise, meaning your part will have straight, parallel outer edges. Curved edges (other than perfect cylindrical profiles) require custom fixtures, costing extra time and money. Thin parts are difficult to hold and are prone to warping.
Design your part for as few setups, or orientations, as possible, i.e. think about how many times your part has to be taken off the mill, rotated, and rejigged. Fewer setups mean less fabrication time, but also fewer inaccuracies!
Harder Materials = Increased Machine Time
Steel, stainless steel, and other hard materials are also slow to machine. Materials like this exponentially increase the time required to machine because every operation is slowed. Substituting a strong, softer material like 6061 aluminum can save you a lot of time and money in the long run.
Non-planar and Draft Angle Surfaces Increase Cost
Non-planar and draft angle surfaces are slow to machine, resulting in more time per part on the CNC machine, and more cost.
Minimize Tool Changes
A tool change is when the CNC machine swaps out cutting tools for a new operation. If you can minimize these tool changes, it will cut down on production time. One example of this is using the same hole size or internal corner radius wherever you can.
Inside Fillets vs Chamfers
Inside chamfers are time consuming and difficult to create. Inside fillets are easier to make because round tipped endmills can be used.
Pro Tip: Place a note on your drawing saying “break all edges” instead of building lots of tiny chamfers on your modeled part. Fictiv will break sharp edges unless otherwise instructed by the customer.
The above best practices will help you create a leaner product with less fabrication time, resulting in less cost. However, some designs may require you to break one of the above best practices—you can always email our prototyping team at firstname.lastname@example.org to make sure the design is machinable.
To check out Fictiv's CNC capabilities, visit our CNC service page.