CNC machining is a marvelous technology that offers a range of possibilities for accurate parts, but your end-product is only as good as the design you set out with. There are some major considerations one has to make when developing any machined part, taking into account its full geometry.
As of yet, such guidelines are more rules of thumb than real protocols set in stone. Industry-wide standards are rare and the technology is always in flux, coming up with new and exciting innovations that push the envelope in terms of what is and isn’t possible. However, there are many practices that have become tried and true rules to live by. Here are some of the restrictions and considerations that come with designing parts for CNC machining.
Generally, it is best to design parts so that tools of the largest diameters possible can machine them. This helps avoid the need for specialist tools and ensures faster processing. It’s also best not to design cavities that are more than four times deeper than their width. It’s vital to make sure the features of the design align with the principal directions your machine allows. This involves keeping in mind the number of axes one is machining with.
When trying to machine text or letters, it is best to use engraved text rather than embossed. Embossed text can end up using a large amount of material that needs to be removed throughout the process. Using a sans serif font with a minimum size of 20 points is also recommended to avoid small, unwanted features within the engraved text.
It’s best to submit a technical drawing when working with a machinist. These need to have a very specific format but can greatly help work through the design of the part and bring out its best qualities.
Before you consider the specifics of the part, it’s important to note the limitations and strengths of the type of CNC machine you have. This may seem basic, but various types of CNC machines offer better control over certain forms and shapes. Some of the most common types are listed below along with their strengths.
- Lathes are commonly used for complex cylindrical shapes. Due its capabilities, the lathe is often the most prominently used for these circular cuts as it offers tight tolerances and a cost-effective level of operation. With lathes, the material turns while the cutting tool remains stationary, so geometries rely on the movement and feed rates of the stationary tools along with the rotational speed control of the material. Lathes are made for turning so shaping is not there biggest forte. Lathes also get less accurate as the material in use gets thicker.
- Milling Machines come in a lot of varieties. The core difference in comparing them to lathes is that the cutting tool moves as opposed to the material. Vertical milling machines have a spindle axis and cutting tool that is aligned vertical to the machines’ bed. Horizontal milling machine cutters are mounted on a horizontal spindle across the table. They are used when a lot of material needs to be removed by the cutters or there is less need for accuracy, in general. Machines with more axes can harness and combine the advantages of both lathes and mills in one set-up.
- Routers are similar to the vertical milling machine in that cutting tools are aligned vertically to the machine’s bed. Additionally, the router also moves about processing the materials, as the part remains fixed in place. The main difference is the work-area-to-machine ratio, which is almost 1:1 for a router but closer to 1:3 for a mill. It is particularly good for large sheets of wood. Design should take into account these differences in area along with how they find inside corners a bit trickier. Similarly, detailed cuts with fine detail will have to use small tools but there’s only so small any tool can get before it becomes ineffective.
One of the most common rules of thumb when it comes to machining is the ratio of tool diameter to cavity depth. The recommended depth of any cavity in your design is four times its width because end mill tools have a limit to their cutting length. This is typically three to four times the diameter of the tool. Lower depth-to-width ratios lead to increased vibration, tool deflection and chip evacuation.
Another common restriction one has to keep in mind is the tool’s geometry. A vast number of CNC cutting and machining tools are cylindrically shaped and can have a restricted cutting length. This shape has a bearing on the final cut that is made. The internal corners of a piece, for example, invariably have a radius. This is true even if you machine them with an extremely small cutting tool.
Specialized tools can help go around some of these problems but they can have their own trade-offs. If the length of the tool is giving you problems in reaching deeper parts of a cavity in the workpiece, can employ a specialized tool with a longer shaft, however the drawbacks need to be kept in mind. Longer tools can increase vibration and reduce the accuracy you are capable of achieving. Part design should typically aim towards employing tools with longer diameters and shorter lengths, as is most feasible for the user.
In designing inner edges, the most commonly recommended vertical corner radius is one-third of the cavity depth or more. In using the recommended corner radii, one should use a diameter tool that follows the suggested cavity depth guidelines. To obtain a surface finish of a higher quality, it is best to have a corner radius slightly higher than the recommended amount. This enables the tool to cut along a circular path, rather than a 90-degree angle. However, if one instead desires a 90-degree angle, it is recommended to use a T-bone undercut (discussed below) rather than opting for a decreased corner radius.
Thin walls can be tricky as decreasing the wall thickness reduces the stiffness of the material, thus increasing vibrations during machining and lowers the achievable accuracy. Additionally, when it comes to plastics and other temperature prone materials, it is best to monitor softening and residual stresses. A larger minimum wall thickness can mitigate these factors. Recommended minimums vary based on materials and tools, but a common guideline machinists work with is 0.8 mm for metals, 1.5 mm for plastics.
With holes, it is best to keep the drilling depth low and not to engage in flat-bottomed holes unless completely necessary, as these can be quite tricky or require specialized tooling. Holes are machined using either a drill bit or an end mill tool and ones with tighter tolerances require finishing using reamers and boring tools. For high accuracy holes with a smaller than 20 mm, using a standard diameter is highly recommended. Holes with non-standard diameters should be machined with an end mill tool. In this case, the maximum cavity depth restrictions apply. Any holes deeper than the typical recommended value of the tool are machined using specialized drill bits (minimum diameter 3 mm).
For extended holes, the part can be drilled from both sides but it’s quite important to recognize that there will be a mismatch where the two holes meet. To counter such a mismatch users can apply jigging.
For edge drilling, one must ensure that the entire diameter of drill is contained within the part. If this is not the case, the drill may break, surface finish could turn out poor and the sharp edge created at the corner is likely to fold. If completely necessary, drill the part first and then mill material away to leave a partial hole.
Threads, Tapping & Thread Milling
Internal threads are usually cut with taps and external threads with dies. Taps and dies can be used to cut threads down. CNC threading tools are common and machinists prefer them because they can limit the risk of tap breakage. There are many different types of taps and each have their own qualities. Cut taps create the female portion of the mating pair by removing material from the hole. With form taps users create thread by displacement of material within the hole. Although both cutting tools and forming tools produce essentially the same thread, and are gaged in the same manner, the requirements for their use, and results achieved, are in many ways different.
Thread mills are another option. These are inserted along the axis of the spindle using helical interpolation to create the thread. Typically taps and thread-mills are for the internal threads and threading dies and thread-mills for the external threads. In terms of speed, a high-speed tapping center set up with a rigid tap can thread holes in a fraction of the time it would take to thread mill the same holes. However, one major limitation of tapping centers is that a different size tap is required for each different size hole.
The brunt of the load that hits a thread hits the few first teeth (up to 1.5 x the nominal diameter). Threads longer than 3x nominal diameter are thus unnecessary. For threads in blind holes cut with taps (i.e. all threads smaller than M6), add an unthreaded length equal to 1.5 x the nominal diameter at the bottom of the hole. When a CNC threading tool can be used (i.e. threads larger than M6), the hole can be threaded throughout its length.
Smaller features can be tough after a certain minimum scale and size. Machining cavities and holes below 2.5 mm (0.1”) in diameter is considered micro-machining, which require specialty tools and expertise. Micro-drills are required to machine such features and the physics of such machining endeavors can be vastly different. It’s best to avoid such features unless absolutely necessary.
Because standard cutting tools must access a piece from directly above, machining undercuts requires the use of specialized tools. There are different design practices for different kinds of undercuts. The two most common ones are T-slot undercuts and Dove-tail undercuts.
Tools for T-slot cutting feature a horizontal cutting blade on a vertical shaft. The undercut’s width can be anywhere from three millimeters to 40 millimeters. It is recommended that you use whole increments or commonly used fractions when defining your undercut width.
Dovetail cutting tools vary based on their angle. The standard angles used are 45 and 60 degrees. You can also, however, find tools of five degrees and 10 degrees on up to 120 degrees in 10-degree increments. If you are designing a part with an undercut on an internal wall, be sure you leave enough clearance room for the tool.
Typically, you will need at least four times the undercut’s depth in between the machined wall and other internal walls. The standard ratio of cutting diameter and the shaft diameter is two to one, which limits the cutting depth. If you need a non-standard depth, machine shops can create custom tools. Keep the undercut amount as small as possible if it is absolutely necessary. However, it’s probably a good idea to avoid undercuts entirely. They can be difficult to machine and complex ones require specialist tooling or multiple setups.
Chamfers & Fillets
A chamfer is a slope cut where two surfaces meet at a sharp edge. This helps ease up assembly for inserting bolts into holes and reduces risk of injury when handling sharp objects. Deburring achieves a similar goal but by breaking the edges of the part. This decreases the size in many instances so chamfering the material is better for specific sizes. Additionally, the edge on a chamfer should be kept at 45° unless it is vital to use another angle.
Fillets require the rounding of an interior or exterior corner of the part. It’s better to keep any radius on the part greater than the cutter radius leading to a more straightforward machining process. Internal fillets, on the other hand, should be as large as possible to allow a large-diameter tool to be used, decreasing machining time. In general, the radius of the internal fillet should be greater than 1/3 of the depth of the cavity to avoid tool-breakage.