Key considerations in CNC machining design and manufacturing

Efficient CNC design is the key to balancing functionality, cost, and production efficiency. By following these guidelines, you can avoid common design challenges, improve manufacturability, and streamline the production process. From minimizing thin walls and deep cavities to setting reasonable tolerances, each recommendation in this solution helps simplify machining and ensure quality.

1. Avoid Excessively Deep Cavities and Grooves

The depth of cavities and grooves is typically related to the diame

ter of the tool used to machine internal fillets. A good rule of thumb is to keep the cavity depth at 3-4 times the tool diameter, or the groove depth less than four times the feature width.

2. Design Larger Internal Fillets

Whenever Possible In CNC machining, any internal cutting will generate a fillet with a radius equal to half the tool's diameter. Milling with smaller tools takes more time, so it is recommended that the fillet radius be greater than one-third of the machining depth. Ideally, the largest possible internal fillets should be designed, and all internal edges should have the same radius so that machining can be completed using the same tool.

If large fillets cannot be used due to design requirements—such as when the part needs to mate with another square component—the following design approach can be adopted to avoid small fillets:

3. Avoid Thin-Wall Structures

Thinwall structures are prone to vibrations during machining, especially when the part features are tall. It is recommended that the minimum thickness for metal thin-wall components be 0.5-0.8mm, while for plastic components, it should be 1.0-1.5mm. If the thick walls are used for support or involve tall features, the wall thickness should be increased appropriately. However, in cases where thin-wall structures must be designed, combining CNC machining with sheet metal riveting processes is a more economical and reasonable choice. Additionally, for thin plate parts with a thickness of 6mm or less, it is advisable to design them to match standard sheet thicknesses that are readily available for purchase.

4. Avoid Deep Holes

For both blind holes and through holes, it is recommended that the hole depth does not exceed four times the hole diameter, with a minimum hole diameter of 1mm. Priority should be given to designing holes with standard sizes. Using standard drill bits allows for efficient and precise hole machining, whereas non-standard holes require end mills, increasing costs. Additionally, blind holes drilled with twist drills will have a 135° conical bottom, while those machined with end mills will have a flat bottom.

5. Use Standard Threads

When designing threads, priority should be given to standard sizes. The larger the thread, the easier it is to machine. The thread length should not exceed three times the hole diameter. For blind hole tapping, it is recommended to leave at least half the hole diameter of extra length at the bottom of the hole. For large-diameter threaded blind holes and threaded bosses, a clearance groove should be reserved at the bottom of the thread to ensure the thread can be fully tightened. Alternatively, consider using inserts such as threaded coils or brass nuts, which are more durable than bare threads, especially in materials like aluminum or plastic, and are easy to install.

6. Reduce the Number of Setups

To reduce machining costs, the number of setups for a part should be minimized. Ideally, all machining can be completed in a single setup. If the part’s structure cannot be machined in the same orientation, multiple setups or the use of multi-axis CNC machines may be required, increasing costs. As shown in the figure below, the part on the left requires two setups to complete machining, while the part on the right can be machined in a single setup.

7. Avoid Non-Functional Aesthetic Features

Non-functional aesthetic designs, such as surface grinding, polishing, anodizing, painting, or electroplating, increase the labor costs associated with post-processing. If not necessary, it is recommended to minimize such designs to reduce machining time and costs.

8. Avoid Designing Overly Small Features

Most CNC machines have a minimum tool diameter of 2.5mm. The smaller the tool diameter, the more prone it is to breaking, requiring micro-cutting and slow feed rates during machining, which increases machining time. Therefore, unless specifically required by the design, overly small features should be avoided. WEIKE CNC machines can accommodate a minimum tool diameter of 0.3mm, enabling the machining of small features with internal corner radii as small as R0.15.

9. Avoid Unmachinable Features

Not all design features can be achieved through CNC machining. For example, holes that are closed at both ends and U-shaped holes cannot be directly machined. A hole closed at both ends must first be machined as a blind hole, and then the top of the hole can be designed with a threaded assembly to close it. U-shaped holes, on the other hand, require disassembly for machining.

10. Avoid Small or Raised Text

When marking part numbers or company names, try to avoid complex text designs. Electrochemical etching or laser engraving is often a better choice. If milling text is necessary, it is recommended to use recessed rather than raised fonts, with a moderate font size and a depth of no more than 0.3mm.

11. Undercut Design

Undercut designs typically come in two types: T-slots and dovetail slots, both of which require the use of T-slot tools for machining. The standard dovetail slot angles are 45° or 60°. During machining, ensure that the width of the top of the T-slot is greater than the diameter of the T-slot tool. The width of the top of the T-slot on the part is typically more than four times the depth of the undercut (as shown in the figure below).

If the T-slot or dovetail slot is a through structure and not within the constraint range, the tool can approach from the side. If the dovetail slot is circular and requires sealing ring assembly, a tool entry point must be set in a specific area of the dovetail slot. The diameter of the tool entry point corresponds to the maximum width at the bottom of the dovetail slot.

11. Avoid External Rounding Corners on Part Edges

To prevent the part from being scratched during handling or assembly, external rounding (R-corner) or a 45° chamfer (C-corner) is typically designed. External R-corners require multiple passes with a ball-end mill or custom internal R-corner tools, while a 45° C-corner can be completed in one pass using a chamfer tool. Therefore, if chamfering is required, it is recommended to prioritize designing a 45° C-corner for part edges.

12. Design Tolerance Ranges Reasonably

For metal parts, unmarked dimensional tolerances typically conform to ISO2768-fH, while for plastic parts, they conform to ISO2768-mK. Excessively tight tolerance requirements increase machining difficulty and time. To optimize production efficiency and cost control, strict tolerances should only be specified when absolutely necessary.

In terms of assembly tolerances, metal parts typically achieve Grade 7, such as H7 for hole-based systems and h7 for shaft-based systems. The smaller the tolerance grade, the higher the precision requirement, and consequently, the greater the machining difficulty.