CNC machining is currently one of the most widely used manufacturing methods. This guide compiles common design considerations for the process. The design principles are:
- The size of the cutting tools used in milling is a critical factor that must be considered when designing a part.
- Always assess whether a cutting tool can physically access and machine any new feature added to the design.
- Fewer fixturing setups reduce machining time and increase accuracy.
- Minimize machining time. Reducing the amount of material removal saves time and cost.
Minimizing Fixturing Setups
The tool path is one of the primary design constraints in CNC machining process. To access all surfaces of the model, the workpiece must be rotated or flipped multiple times. Each time the workpiece is rotated, the machine datum must be recalibrated and a new coordinate system defined.
Limiting the number of setups during design is important for 2 main reasons:
Setup count affects cost: Rotating and recalibrating the part datum requires manual intervention, which increases the total processing time. While three or four rotations may be acceptable, any excessive number of setups adds unnecessary cost.
Setup count harms accuracy: To achieve the maximum relative positional accuracy between two or more features, those features must be machined in the same setup. Introducing a new calibration step adds a small but unavoidable error, regardless of the precision of the fixture. More setups directly compromise final accuracy.
Deep Slot Design
Deep and narrow slots require the use of longer cutting tools. Long tools are more prone to breakage and can introduce tool chatter or machine vibration. Furthermore, machining a deep slot requires multiple passes, which increases machining time and manufacturing cost.
Avoid designing parts with deep slots whenever possible. If unavoidable, the depth should be minimized, or the cross-sectional area of the slot should be increased. Generally, the slot depth should not exceed 3 times the tool diameter. For example, a 6mm tool should not cut a slot deeper than 18mm. Engineers may need to adjust this ratio based on the specific material and available tooling.
Narrow or Constrained Areas
Narrow areas are difficult to machine because the tool size is constrained by the minimum distance between the feature’s faces. Long, small-diameter tools are susceptible to breakage and chatter. Avoid designing features that are too narrow for the tool to pass through easily. If narrow areas are necessary, they should not be deep; remember that the cutting depth for any feature should generally be less than 3 times the tool diameter.
Cavities
It is recommended that the cavity depth be less than 4 times the cavity width.
End mills have limited cutting lengths (typically 3 to 4 times their diameter). When a pocket has a large depth-to-width ratio, tool deflection, chip evacuation issues, and vibration become more pronounced. Limiting the cavity depth to within four times its width ensures consistent results. If greater depth is required, consider designing the part with variable cavity depths.
Deep Cavity Milling: A cavity deeper than six times the tool diameter is considered a deep pocket. Using specialized tooling, a depth-to-diameter ratio of up to 30:1 may be feasible.
Internal Sharp Corners and Chamfers
Internal sharp corners are impossible to achieve with standard milling, as all milling tool heads have a circular profile when rotating. Instead, the milling cutter leaves an unmachined area (a corner radius) equal to the radius of the tool used. While alternative methods like electrical discharge machining can create internal sharp corners or square internal pockets, these methods are often expensive.
The size of the cutting tool used is a key consideration. Larger tools remove more material per pass, reducing machining time and cost. A technique to improve efficiency is to make the corner radius slightly larger than the end mill’s radius. A corner radius 0.1mm larger than the standard tool radius will create a smoother cutting path and a finer finish on the part.
To maximize the advantage of using larger tools, design the largest possible radius for internal corners, ideally greater than 0.8mm. Excluding micro-machining applications, using a corner radius greater than 3mm (where space permits) and maintaining the largest possible tool diameter will improve efficiency and tool stability.
| Parameter | Recommended |
| Internal Radius | At least > 1/3 of the depth |
If a straight corner is required, an alternative design using a relief cut can be implemented. It is worth noting that using a drill bit instead of an end mill at the corner can achieve a smaller radius and the necessary depth.
Fillets vs. Chamfers on External Edges
External fillets—rounded edges on bosses, slots, and the tops of features—require specialized, sharp tooling that matches the radius, both of which can be costly. To avoid these expenses, design a chamfer (beveled edge) on the feature’s external edges instead of a fillet, unless a fillet is strictly required.
It is important to note that burrs are an unavoidable byproduct of machining sharp edges, and a chamfering step is necessary, especially on the main external perimeter of the part, to prevent operator injury.
Tool Accessibility
Always ensure the cutting tool can access all features within the part without being obstructed by other features.
If dovetail or T-slots are necessary, it is recommended to consult a specific design guide for these features. Dovetail and T-slots require specialized cutters and should be avoided unless they are necessary for the application.
Thin Walls
When milling metal, thin walls increase the risk of chatter, which negatively impacts machining accuracy and surface finish. For plastics, thin walls can lead to warping and softening.
It is critical to avoid designing parts with thin walls. As a practical minimum, wall thicknesses of approximately 0.8mm for metal and 1.5mm for plastic are achievable.
To avoid complications, a wall thickness greater than 1.5mm to 2mm is generally necessary for metal parts, and greater than 2mm for plastic parts. Achieving thinner cross-sections without significant risk is possible but requires a case-by-case assessment.
Flat-Bottomed Holes
Machining flat-bottomed holes requires more expensive processes and can lead to issues in subsequent operations, such as reaming. Avoid creating flat-bottomed blind holes, especially small ones, and instead design holes with a standard twist-drill point. The standard drill point angle is 118°.
It must be emphasized that the hole model should be designed with the conical bottom shape from the start—this is not a difficult modeling step, rather than shifting the problem to manufacturing.
Optimal Hole Diameter and Depth
Holes can be machined using drill bits or end mills. Drill bit sizes are standardized (metric and imperial). Reamers and boring tools are used for finishing holes that require tight tolerances.
For high-precision holes with a diameter less than 20mm, use standard drill diameters. Non-standard diameters must be machined with an end mill; in this case, the hole depth should be kept within pocket depth limitations, adhering to the maximum recommended depth values.
| Parameter | Recommended (mm) | Feasible (mm) |
| Minimum Hole Diameter | 2.5mm | 0.05mm |
In most cases, tools with a diameter less than 2.5mm can accurately machine cavities and holes. Anything below this limit is considered micro-machining, which requires specialized micro-drills and expertise. Therefore, it is advisable to avoid micro-machining unless necessary.
There is no preference between through-holes and blind holes in CNC milling. On non-CNC milling machines, through-holes tend to be simpler to machine than blind holes.
Start Your Production From Prototyping to Scale
- Reliable, On-time Global Delivery
- Multiple Certifications Available
- Full Inspection Before Every Shipment
Hole Depth
Design the shortest hole depth necessary. Deep hole drilling systems can machine very deep holes, but this requires specialized equipment and tooling.
| Parameter | Recommended | Feasible |
| Hole Depth | 4 times Diameter | 40 times Diameter |
Threaded Hole Design
Internal threads can be machined using a tap or a thread mill. Taps are used for threads M2 and larger. CNC thread mills can machine threads as small as M6.
| Parameter | Minimum Thread Length (mm) | Recommended (mm) |
| Thread Length | 1.5 times Diameter | 3 times Diameter |
Most of the load applied to a thread is carried by the first few turns near the hole, opening up to 1.5 times the diameter. Therefore, a thread length greater than 3 times the nominal diameter is generally unnecessary. For threads in blind holes machined with a tap (i.e., all threads smaller than M6), add a non-threaded length equal to 3 times the pitch at the hole bottom to accommodate the tap’s lead section. When thread milling is used (i.e., threads larger than $M6$), the hole can be threaded along its entire length by designing a relief groove.
Avoiding Deep Tapping
To ensure accurate and precise results, avoiding deep tapping is critical in CNC design. Longer tap depth increases the risk of vibration and misalignment during the operation, leading to product defects. Threads exceeding 3 times their diameter are considered deep and pose a risk. However, in many cases, a thread length of even $1.5$ times the diameter provides sufficient thread engagement, often eliminating the need for deep tapping. Using deep taps increases the risk of tool breakage, thread defects, and reduced accuracy, making it an undesirable design aspect.
Tool Entry and Exit
When a drill bit contacts a surface that is not perpendicular to its axis, the drill tip will drift. Furthermore, an uneven exit burr around the exit hole will make deburring difficult. Avoid designing hole features with start and end faces that are not perpendicular to the drill’s axis.
If a non-ideal hole orientation is necessary, a small flat surface (spot face) should be designed to provide a perpendicular starting platform.
Avoiding Non-Planar and Drafted Surfaces
Non-planar (complexly curved) and drafted surfaces are challenging to machine, which can result in slower feed rates, longer processing times, and increased tool wear. These surfaces also make it harder to achieve consistent part quality and tight tolerances.
Draft angles are mandatory for parts requiring mold manufacturing, but should be avoided for other parts. To avoid non-planar and drafted surfaces in your design:
- Aim to use simple, flat geometries whenever possible.
- Use fillets and radii to soften sharp corners and minimize the number of complex surfaces.
About Getzshape
We don’t just machine parts, we engineer solutions. Our experienced team integrates deep DFM analysis into every project, bridging the gap between design intent and manufacturing reality. Contact us today to review your design and make it a tangible shape.
