Overview
CNC machining involves using high-speed rotating cutting tools to remove material from a solid block in order to fabricate the desired part according to the drawing. The cutting tool plays a crucial role in CNC machining as it directly contacts the part and removes excess material to achieve the required shape.
Common CNC cutting tools, such as end mills and drills, have cylindrical shanks with specific tip shapes and limited cutting lengths. These two characteristics of the tools limit their cutting capabilities, making it difficult to machine deep, small holes and undercuts. Here are some commonly used cost-saving design tips:
I. Considerations for Minimum Radius Corners
CNC milling cutters have a cylindrical shape. When cutting internal walls, a radius will appear at the vertical corners. Small tools can make multiple passes at a lower speed to achieve a small radius, but this will result in more time and higher costs.
Therefore, when designing parts to be manufactured by CNC machining, it is advisable to increase the radius of the cavity depth and use a similar radius for internal edges. If you do not provide a 2D drawing with special instructions to remove the radius at the right angles, our company will machine all internal cavity right angles with the minimum R according to the following rules:
Assume the tool diameter is ∮D mm, the maximum depth of the internal cavity is H mm, and the minimum internal R is R. The formula is R = (H/10) + 0.5, and ∮D = H/5. For example, if the internal cavity depth is 30 mm, the minimum internal R that can be machined is R3.5 mm = (30/10) + 0.5, and the corresponding tool is ∮6 = 30/5. Currently, we can achieve a minimum internal R of R0.5 with a depth ≤ 3 mm. The smaller the internal R, the smaller the tool required, and the higher the machining cost.
We recommend making the R corners as large as possible when feasible!
If you need the part to retain right angles, please provide a 2D drawing with annotations. You can opt for EDM (Electrical Discharge Machining) to remove the radius (which requires CNC machining of a copper electrode followed by EDM processing, resulting in higher costs), or modify the part structure to create an R corner relief, which can be directly machined by CNC at a lower cost. If the part has through-holes on both sides, wire cutting can be used to remove the radius, but this also incurs higher costs.
II. Considerations for Threads
To reduce communication costs and avoid machining errors, it is recommended to design threads according to standard drill inner diameters and thread rolling outer diameters, and to fully describe the thread parameters. When placing orders, try to include both internal and external threaded parts in the same order for processing.
Each engineer may draw the thread bottom hole diameter differently in 3D drawings. For example, the standard bottom hole diameter for an M3x0.5 thread is ∮2.5 (see the figure below). In programming, the bottom hole is drilled directly according to ∮2.5, and then tapped using an automatic tapping machine. If the bottom hole is drawn as ∮3, it will be too large for tapping (although some cases can be remedied by inserting a thread insert).
For special threads, provide a physical sample for fitting.
Strong thread connections occur in the first few threads. Sometimes, a very long thread length is not necessary at all. Long thread holes may require special tools and more machining time and cost. It is recommended that the thread length not exceed 3 times the hole diameter. For blind thread holes, it is advisable to leave a thread-free length of at least half the hole diameter at the bottom of the hole.
III. Considerations for Cavity Depth
Machining deep cavities significantly impacts the cost of CNC parts because a large amount of material needs to be removed, which is extremely time-consuming. CNC cutting tools have limited cutting lengths and perform best when the cutting depth is 2-3 times their diameter. For example, a ø12 milling cutter can safely cut cavities up to 25 mm deep.
Cutting deeper cavities (5 times the tool diameter or more) can lead to tool overhang, tool deflection, chip evacuation difficulties, and tool breakage. Therefore, special tools or multi-axis CNC systems are required. Additionally, when cutting cavities, the tool must be tilted to the correct cutting depth, and a smooth entry requires sufficient space.
Limiting the depth of all cavities to 5 times their length (i.e., the maximum dimension in the XY plane) can achieve minimum machining costs.
IV. Considerations for Thin Wall Thickness
Thin wall machining requires multiple passes at a low cutting depth and is prone to vibration, resulting in deformation or breakage. Therefore, thin walls are difficult to machine accurately and increase machining time.
For metal parts, the wall thickness should preferably be designed to be more than 0.8 mm (minimum achievable thickness is 0.5 mm), and for plastic parts, the minimum wall thickness should be more than 1.5 mm (minimum achievable thickness is 1 mm).
V. Considerations for Tolerances
Tighter tolerances increase machining and quality inspection time, resulting in higher costs.
If no specific tolerance is indicated on the part drawing, the part will be machined according to standard tolerances (±0.1 mm or higher). If there are special tolerance requirements, be sure to provide a 2D drawing with corresponding annotations.
VI. Considerations for 2D Drawings
2D drawings are the best way to convey certain aspects of a design. Clearly annotate tolerances, surface roughness, assembly methods, and key inspection points and quality control requirements on critical features. This provides a reference for selecting the best machining method and process route, resulting in lower costs.
Also, annotate thread holes and dimension depths accordingly.
Engineering drawing review will compare the 3D and 2D drawings, and any conflicts can be promptly communicated and resolved.
