Design Guide: Computer Numerical Controlled (CNC) Machining
Last Updated: July 25th, 2018
Table of Contents:
Computer Numerical Controlled (CNC) Machining is a means to remove material using high speed, precision machines that use a wide variety of cutting tools to create the final design. Common CNC machines include vertical milling machines, horizontal milling machines, and lathes.
To successfully make a part on a CNC Machine, programs instruct the machine how it should move. The programmed instructions given to the CNC machine are encoded using CAM (computer aided manufacturing) software in conjunction with the CAD (computer aided design) model provided by the customer. The CAD model is loaded into the CAM software and tool paths are created based on the required geometry of the manufactured part. Once the tool paths are determined, the CAM software creates machine code that tells the machine how fast to move, how fast to turn the stock and/or tool, and where to move in a 5-axis X, Y, Z, A and B coordinate system.
Complex cylindrical shapes can be manufactured more cost effectively using a CNC lathe versus a 3 or 5-axis CNC milling machine. With a CNC lathe, the part stock turns while the cutting tools remain stationary. Conversely, on a CNC mill, the cutting tools move while the stock remains fixed. To create the geometry of a part, the CNC computer controls the rotational speed of the stock as well as the movement and feed rates of the stationary tools. If square features are needed on an otherwise round part, the round geometry is first created on the CNC lathe followed by the square features on a CNC mill.
Because the computer controls the machine movement, the X, Y, and Z axes can all move simultaneously to create everything from simple straight lines to complex geometric shapes. However, despite advancements in tooling and CNC controls, some limitations do still exist in CNC Machining and not all shapes and features can be created. These limitations will be discussed in this guide.
Tolerance is the acceptable range for a dimension which is determined by the designer based on the form, fit and function of a part. Unless specifically called out by the designer, the standard tolerance used by Xometry is +/-.005” for metal parts and +/-.010” for plastic parts. If tighter tolerances (less than the standard, e.g. +/-.002”) are required, information regarding which dimensions require the tighter tolerances must be communicated to Xometry. As a point of reference, a piece of paper is about 0.003” thick.
It is important to keep in mind that a tighter tolerance can result in additional cost as a result of increased scrap, additional fixturing, special measurement tools and/or longer cycle times (the machine may need to slow down in order to hold the tighter tolerance). Depending on the tolerance call out and geometry associated with it, the part cost can be more than double what it would be with a standard tolerance.
Overall geometric tolerances can also be applied to the drawing for the part. Based on the geometric tolerance and type of tolerance applied, additional costs may be incurred due to the additional inspection time required.
To help minimize cost, to only apply tight and/or geometric tolerances to critical areas.
Xometry’s lathe capabilities allows for successful machining of parts up to 18” (457.2mm) in diameter, but special cases may be made for larger parts. Xometry is capable of utilizing a live tooling lathe, which dramatically decreases lead times and increases the amount of features that can be machined.
Xometry offers the following plastics for CNC Machining:
- Acetal (Delrin®)
- Other custom plastics
Plastic can be a less expensive alternative to metal if a part’s design does not require the rigidity of metal. Polyethylene, for example, is easy to machine and is about 1/3 the cost of 6061 aluminum. In general terms, ABS is about 11/2 times the cost of acetal, while nylon and polycarbonate are approximately 3 times the cost of acetal.
Note: Depending on a part’s geometry, tight tolerances can be harder to hold with plastics. Parts may also warp after machining as a result of the stress created when material is removed.
Complexity & Limitations
CNC Machining can effectively produce both simple and complex designs. The more complex the part—i.e. a part with contoured geometry or multiple faces that need to be cut—the more costly it becomes due to the additional setup and machining time required. When a part only requires one setup and 3 axes (for example X and Y, and the tool movement making Z), the setup and machining can be accomplished faster, thus minimizing the cost.
To create a complex surface with a suitable surface finish, very small cuts are made. These small cuts take significantly longer to machine than larger cuts on broader or planar geometries, which in turn increases the cost. To help minimize cost and machining time, try to design parts using on-axis planes possible. Keeping features such as internal corner radii and tapped holes consistent will also help save time and money on parts by reducing the need for tool changes.
When using a CNC vertical or horizontal milling machine, all interior vertical walls will have a radius. This is because material is removed with a round tool spinning at high RPMs. Part designs must take into account areas where radii will occur as a result of this limitation.
Inside Corner Fillets
For internal corner radii, it may be better to use a non-standard radius. This is because endmills need clearance to turn and continue milling when tracing the internal corner (see Fig. 1).
If a part features a 0.25” interior radius, the standard endmill would need to hammer the corner, come to a complete stop, pivot 90 degrees, and then resume cutting. Doing this slows down machining speed (creating additional cost), and also causes vibration (creating chatter marks). By adding 0.02” (0.508mm) - 0.05” (1.27mm) to internal radii, the cutter will be able to turn slightly without coming to a complete stop. This will not only reduce the part’s cost, it will also improve the part overall (see Fig. 2).
The larger the radius, the lower the cost—larger tools can be used to machine larger parts, resulting in more material being removed with each cut, which in turn reduces machining time. For example, in the illustration to the right (see Fig. 3), using a tool with a 0.125” diameter (0.063” radius) would take approximately 11/2 times longer than using a 0.187” diameter tool and approximately 2 times longer than a 0.250” diameter tool.
Though small radius tools (down to a .015” radius) are available, sometimes the depth of cut required makes the cut impossible because the tool is not manufactured. If the tool is manufactured, the part cost will increase significantly as a result of the increased manufacturing time required to machine a part using only small cuts.
When the depth of cut becomes greater than 2 times the diameter of the cutting tool, the tool’s feed rate must slow down, which increases the cycle time and part cost. For every doubling of the length of cut, feed rate is more than halved, which more than doubles the time to cut the feature. he maximum cut depth to tool diameter ratio is 4 times for pockets and 10 times for drilled or reamed holes. Ratios greater than this may require special tooling. For example, using a 0.125” diameter tool, the max cut depth would be 0.50” and drill depth is 1.25” before a custom tool would be required.
Some features cannot be reached by a standard machining tool, thus creating an undercut region on the part. Care must be taken when designing an undercut for two reasons:
First, if the feature is not a standard dimension, the undercut may require the creation of a custom tool. In the example at right (Fig. 1), the radius in the slot is 0.053”. A costly custom tool would be necessary to create the geometry, causing part cost to increase significantly— especially if only a few parts are to be manufactured. If a standard .062” radius were to be used, then the tool’s cost would be less than half that of a custom tool.
Second, there are limits to the depth of cut due to the construction of the tool (a horizontal cutting blade attached to a vertical shaft). There is no “standard depth” for undercuts, but the shallower the better. Designing undercuts in accessible places is also critical. The illustration at right (Fig. 2), for example, depicts an undercut feature that cannot be reached in the machining process.
Other types of finishes, including iridite, are available upon request. Submit an RFQ and we’ll look into a finishing process for you.