In order to make full use of the ability of CNC machining, designers must follow specific manufacturing rules. But this can be a challenge because there is no specific industry standard. In this article, we have compiled a comprehensive guide with best design practices for CNC machining.
We focus on describing the feasibility of modern CNC systems, ignoring the related costs. For guidance on designing cost-effective parts for CNC, please refer to this article.
CNC machining
CNC machining is a subtractive machining technology. In CNC, various high-speed rotating (thousands of RPM) tools are used to remove materials from solid blocks to produce parts according to CAD models. Metal and plastic can be processed by CNC.
CNC machining parts have high dimensional accuracy and strict tolerance. CNC is suitable for mass production and one-time work. In fact, CNC machining is currently the most cost-effective way to produce metal prototypes, even compared to 3D printing.
Main design limitations of CNC
CNC provides great design flexibility, but there are some design limitations. These limitations are related to the basic mechanics of the cutting process, mainly related to tool geometry and tool access.
1. Tool geometry
The most common CNC tools (end mills and drills) are cylindrical with limited cutting length.
When the material is removed from the workpiece, the geometry of the tool is transferred to the machined part. This means that, for example, no matter how small a tool is used, the internal angle of a CNC part always has a radius.
2. Tool access
In order to remove the material, the tool approaches the workpiece directly from above. Functions that cannot be accessed in this way cannot be CNC processed.
There is one exception to this rule: undercut. We will learn how to use undercuts in design in the next section.
A good design practice is to align all features of the model (holes, cavities, vertical walls, etc.) with one of the six main directions. This rule is considered a recommendation, not a limitation, because the 5-axis CNC system provides advanced workpiece holding capability.
Tool access is also an issue when machining features with large aspect ratios. For example, to reach the bottom of the deep cavity, a special tool with a long axis is required. This reduces the stiffness of the end effector, increases vibration and reduces achievable accuracy.
CNC experts recommend designing parts that can be machined with tools with the maximum possible diameter and the shortest possible length.
CNC design rules
One of the challenges often encountered when designing parts for CNC machining is that there is no specific industry standard: CNC machine tool and tool manufacturers constantly improve their technical capabilities and expand the range of possibilities.
In the following table, we summarize the recommended and feasible values of the most common features encountered in CNC machining parts.
1. Cavity and groove
Recommended cavity depth: 4 times cavity width
The cutting length of the end mill is limited (usually 3-4 times its diameter). When the depth width ratio is small, the tool deflection, chip discharge and vibration become more prominent. Limiting the depth of the cavity to four times its width ensures good results.
If a greater depth is required, consider designing a part with a variable cavity depth (see the figure above for an example).
Deep cavity milling: a cavity with a depth greater than 6 times the tool diameter is considered as a deep cavity. The ratio of tool diameter to cavity depth can be 30:1 by using special tools (using end mills with a diameter of 1 inch, the maximum depth is 30 cm).
2. Inner edge
Vertical corner radius: recommended ⅓ x cavity depth (or greater)
Using the recommended value of the internal corner radius ensures that the appropriate diameter tool can be used and aligned with the guidelines for the recommended cavity depth. Increasing the corner radius slightly above the recommended value (e.g. by 1 mm) allows the tool to cut along a circular path instead of a 90 ° angle. This is preferred because it can obtain a higher quality surface finish. If an internal angle of 90 ° sharpness is required, consider adding a T-shaped undercut instead of reducing the angle radius.
The recommended bottom plate radius is 0.5mm, 1mm or no radius; Any radius is feasible
The lower edge of the end mill is a flat edge or a slightly round edge. Other floor radii can be processed with ball head tools. It is a good design practice to use the recommended value because it is the first choice of the machinist.
3. Thin wall
Recommended minimum wall thickness: 0.8mm (metal) and 1.5mm (plastic); 0.5mm (metal) and 1.0mm (plastic) are feasible
Reducing the wall thickness will reduce the stiffness of the material, thereby increasing the vibration in the machining process and reducing the achievable accuracy. Plastics tend to warp (due to residual stress) and soften (due to temperature rise), so it is recommended to use a larger minimum wall thickness.
4. Hole
Diameter recommended standard drill size; Any diameter greater than 1mm is acceptable
Use a drill or end mill to machine holes. Standardization of drill bit size (metric and English units). Reamers and boring cutters are used to finish holes requiring strict tolerances. For sizes less than ▽ 20 mm, standard diameters are recommended.
Maximum depth recommended 4 x nominal diameter; Typically 10 x nominal diameter; 40 x nominal diameter where feasible
Non standard diameter holes must be processed with end mills. In this case, the maximum cavity depth limit applies and the recommended maximum depth value should be used. Use a special drill (minimum diameter 3 mm) to machine holes with a depth exceeding the typical value. The blind hole machined by the drill has a conical bottom plate (135 ° angle), while the hole machined by the end mill is flat. In CNC machining, there is no special preference between through holes and blind holes.
5. Thread
The minimum thread size is m2; M6 or larger is recommended
The internal thread is cut with a tap, and the external thread is cut with a die. Taps and dies can be used to cut threads to m2.
CNC threading tools are common and preferred by machinists because they limit the risk of tap breakage. CNC thread tools can be used to cut threads to M6.
The minimum thread length is 1.5 x nominal diameter; 3 x nominal diameter recommended
Most of the load applied to the thread is borne by a few first teeth (up to 1.5 times the nominal diameter). Therefore, no more than 3 times the nominal diameter of the thread is required.
For threads in blind holes cut with a tap (i.e. all threads smaller than M6), add a non threaded length equal to 1.5 x nominal diameter at the bottom of the hole.
When a CNC thread tool can be used (i.e. the thread is larger than M6), the hole can run through its entire length.
6. Small features
The minimum hole diameter is recommended to be 2.5 mm (0.1 inch); 0.05 mm (0.005 in) is feasible
Most machine shops will be able to accurately machine cavities and holes using tools less than 2.5 mm (0.1 inch) in diameter.
Anything below this limit is considered micromachining. Special tools (micro drills) and expert knowledge are required to process such features (the physical changes in the cutting process are within this range), so it is recommended to avoid using them unless absolutely necessary.
7. Tolerance
Standard: ± 0.125 mm (0.005 in)
Typical: ± 0.025 mm (0.001 in)
Feasible: ± 0.0125 mm (0.0005 in)
Tolerances define the boundaries of acceptable dimensions. The achievable tolerances depend on the basic dimensions and geometry of the part. The above values are reasonable guidelines. If no tolerance is specified, most machine shops will use a standard ± 0.125 mm (0.005 in) tolerance.
8. Words and lettering
The recommended font size is 20 (or larger), 5mm lettering
Engraved characters are preferably embossed characters because less material is removed. It is recommended to use sans serif fonts (such as Arial or Verdana) with a size of at least 20 points. Many CNC machines have pre programmed routines for these fonts.
Machine settings and part orientation
The schematic diagram of parts that need to be set several times is as follows:
As mentioned earlier, tool access is one of the main design limitations of CNC machining. To reach all the surfaces of the model, the workpiece must be rotated several times.
For example, the part of the above image must be rotated three times in total: two holes are machined in two main directions, and the third enters the back of the part.
Whenever the workpiece rotates, the machine must be recalibrated and a new coordinate system must be defined.
It is important to consider the machine settings in design for two reasons:
The total number of machine settings affects costs. Rotating and realigning parts requires manual operation and increases the total processing time. If the part needs to be rotated 3-4 times, this is generally acceptable, but any exceeding this limit is redundant.
In order to obtain maximum relative positional accuracy, two features must be machined in the same setup. This is because the new call step introduces a small (but not negligible) error.
Five axis CNC machining
When using 5-axis CNC machining, the need for multiple machine settings can be eliminated. Multi axis CNC machining can manufacture parts with complex geometry because they provide 2 additional rotational axes.
Five axis CNC machining allows the tool to always be tangent to the cutting surface. More complex and efficient tool paths can be followed, resulting in better surface finish and lower machining time.
Of course, 5-axis CNC also has its limitations. The basic tool geometry and tool access restrictions still apply (for example, parts with internal geometry cannot be machined). In addition, the cost of using such systems is higher.
Design undercut
Undercuts are features that cannot be machined with standard cutting tools because some of their surfaces cannot be directly accessed from above.
There are two main types of undercuts: T-grooves and dovetails. Undercut can be single-sided or double-sided and processed with special tools.
The T-groove cutting tool is basically made of a horizontal cutting insert connected to a vertical axis. The width of the undercut may vary between 3 mm and 40 mm. It is recommended to use standard dimensions for widths (i.e., full millimeter increments or standard inch fractions) as tools are more likely to be available.
For dovetail tools, the angle defines the feature size. 45 ° and 60 ° dovetail tools are considered standard.
When designing parts with undercuts on the inner wall, remember to add enough clearance for the tool. A good rule of thumb is to add at least four times the undercut depth between the machined wall and any other inner wall.
For standard tools, the typical ratio between the cutting diameter and the shaft diameter is 2:1, which limits the cutting depth. When non-standard undercut is required, the machine shop usually makes customized undercut tools by itself. This increases lead times and costs and should be avoided as much as possible.
T-shaped groove (left), dovetail groove undercut (middle) and unilateral undercut (right) on the inner wall
Drafting technical drawings
Note that some design criteria cannot be included in step or IGES files. If your model contains one or more of the following, 2D technical drawings must be provided:
Threaded hole or shaft
Tolerance dimension
Specific surface finish requirements
Instructions for CNC machine tool operators
Rule of thumb
1. Design the parts that can be processed with the largest diameter tool.
2. Add large fillets (at least ⅓ x cavity depth) to all internal vertical angles.
3. Limit the depth of the cavity to 4 times its width.
4. Align the main functions of the design along one of the six main directions. If this is not possible, 5-axis CNC machining can be selected.
5. When your design includes thread, tolerance, surface finish specification or other comments of the machine operator, please submit technical drawings with the drawings.
