How to Reduce CNC Machining Costs

A CNC machining tool – such as an end mill or milling cutter – will automatically leave rounded inside corners. The wider this radius, the less passes that the tool will need to make to remove material.

By contrast, a narrow inside corner radius requires both a small tool to machine away material and more passes — often at slower speeds to reduce the risk of deflection or tool breakage — resulting in more machining time.

For optimum design, use an inside corner radius that has a L:D ratio (length to diameter) of 3:1 or less. In addition, try to keep internal corner radii the same, if possible. This helps eliminate tool changes, which adds complexity and can increase run time significantly.

Parts with deep internal cavities are often time-consuming and expensive to manufacture.

The reason is that these designs call for fragile tools that are susceptible to breaking during machining.

To avoid this, either an end mill must be progressively “stepped down” in smaller and smaller increments to reach the desired specs, or other forms of machining, such as broaching or a wire EDM can be used; however, these can be just as costly.

As a best practice, we suggest parts with lengths up to 4X their depth. Anything greater than that becomes exponentially more expensive to manufacture.

Typically, only a few surfaces of a part are critical to its function. The more features with numerical callouts in the design (e.g., radii, hole diameters and chamfers), the more expensive a part becomes to manufacture.

In order to eliminate unnecessary costs, the key is to only assign numerical values to mission critical features and surfaces. Other, less significant features should be controlled by the model (standard tolerance of +/- 0.005″).

Also, try to define a single datum, like the intersection of two sides or the center of a hole, and then dimension everything else from this.

At Xometry, our typical tolerance accuracy ranges from 0.005″ – 0.001″, depending on customer specs.

CNC parts with thin walls have a tendency to chatter, which slows down machining speeds. They can also cause distortion, which makes it difficult to hold tolerances. The result can be additional costs.

In order to keep machining costs low, thin walls should have a minimum width of 1/32” (0.794mm).

If very thin walls are needed, it’s usually more economical to utilize other manufacturing methods, such as sheet metal fabrication.

When it comes to tapped holes, two factors that can add cost are hole depth and tap size.

Typically, increasing the length of thread in a hole does little to hold the bolt tighter. It’s really just the first two or three turns that do all the work. As a result, you don’t need to thread a hole to more than 3X the hole’s diameter (and keep it shorter, if possible). Going deeper just increases the risk of tap breakage and adds time to the tapping operation.

In addition, utilizing standard tap sizes can help cut down on costs. For example, 4-40 taps are more common and generally available than 3-48 taps. In the same vein, avoid very small threaded holes, if possible. Anything smaller than a 2-56″ requires hand tapping, which adds significant time and risk to the process.

Keep hole sizes to standard fractional, number or letter drill sizes. That way, you won’t need end mills or reamers to finish the hole size to a non-standard dimension. This helps reduce machine time to keep costs down.

If you aren’t familiar with drill and end mill sizes, it’s safe to assume that conventional fractions of an inch, like 1/8”, 1/4”, or whole numbers of millimeters will be “standard.” Avoid using measurements like 0.492” or 3.841 mm.

In general, softer metals are less expensive to machine than harder materials for a few reasons:

• In most instances, the raw material is more economical.
• Softer materials, e.g., aluminum 6061, cut more easily, which means less machining time.
• Harder materials require more expensive tools, and are more likely to break and wear tools, which can add to the project cost.

If a material like aluminum 6061 is too soft for your parts, look for a more machinable mild steel instead.

This applies to surface roughness or texture, and appearance-altering finishes like chem film, (sometimes called chromate,) or anodizing.

Mixing and matching adds a lot of cost. For example, requesting a mixture of anodized and chem film finishes on a part adds several processing steps. The same applies when specifying a smooth finish in one area and a bead blast finish elsewhere.

In terms of surface smoothness, it is best to either leave it open or request a uniform finish. If in doubt, it helps to explain the part’s function to your project manager.

In some cases, complex parts would be less expensive if they’re designed and machined as separate parts, and then welded or bolted together afterward.

This is especially true for parts with deep pockets, which would require hours of machining time to remove material, plus additional material costs.

It’s also true for parts that require operations on multiple faces, which can add to fixturing and setup times.

Although modern CNC milling machines can combine multiple operations to run efficiently, they still need programming and setup.

Ordering multiple quantities of the same part helps generate production efficiencies and lower the cost per piece.

At the production phase (up to 10,000 parts), CNC machining can provide maximum cost-efficiency.