14 proven design tips to reduce the cost of CNC machining

In CNC machining, whether you are producing a single prototype or scaling to large volumes, reducing manufacturing cost is often the priority. Design choices can help keep pricing down. By following design for machinability (DFM) guidelines, you can manufacture cost effective parts that still meet functional performance requirements. 

This article provides practical tips to optimize your design. It starts by outlining the main cost drivers in CNC machining, then presents proven guidelines to reduce your project cost. 

How much does CNC machining cost?

A quote for CNC machined parts is determined by several factors: 

• Machining time: Longer cycle times increase cost. Machining time is often the primary cost driver in CNC, especially for high volume production where small design issues can reduce economies of scale. 

• Start-up costs: These include computer-aided design (CAD) file preparation and process planning. They are significant at low volumes but are fixed costs. If the design and surface finish scale well, you can reduce unit price by leveraging economies of scale. 

• Other manufacturing costs: Specifying tight tolerances or designing features that are difficult to machine, such as very thin walls, may require special tooling, tighter quality control, and additional operations at lower cutting speeds. These factors increase total machining time and overall cost.

• Material cost: Raw material price and machinability strongly influence overall cost. Selecting a machinable material and optimizing design for minimal waste can reduce expense.

Understanding CNC machining cost drivers helps engineers optimize designs and lower total cost, especially for outsourced production. 

How to reduce CNC machining cost

1. Add a radius in internal vertical edges

All CNC milling tools are cylindrical and leave an internal radius at pocket corners. Reducing the corner radius requires a smaller diameter tool, which needs multiple passes at lower speed because smaller tools remove less material per pass. This increases machining time and cost. 

To minimize cost:

• Specify a corner radius of at least one third of the cavity depth; larger radii are better.

• Use the same radius for all internal edges to eliminate tool changes. 

• At the cavity floor, apply a small radius (0.5 or 1 mm) or none. 

Good to know: The corner radius should be slightly larger than the cutter radius to lower tool load and reduce cost. For example, for a 12 mm deep cavity, specify a 5 mm or larger corner radius. This allows an 8 mm diameter tool to run at higher speeds. 

Pro tip: When sharp internal corners are required, for example to fit a rectangular part in a cavity, add reliefs or undercut features rather than reducing the internal corner radius, as shown below. 

2. Limit the depth of cavities

Machining deep cavities increases CNC part cost because large amounts of material must be removed, which is time consuming and wasteful.  

CNC tools have limited cutting length and work best when cavity depth is about two to three times the tool diameter. For example, a 12 mm end mill can safely cut cavities up to about 25 mm deep. Deeper cuts, up to four times the diameter or more, are possible but raise cost because special tooling or multi-axis CNC systems are required. 

To minimize cost:

• Limit cavity depth to no more than four times the feature length, defined as the largest dimension in the XY plane. 

• Adjust internal corner radii accordingly and refer to tip 1 if needed. 

3. Increase the thickness of thin walls

Unless weight is a primary concern, thicker solid sections are more stable and less expensive to machine. When thin walls are required, multiple passes at low cutting depths are used to reduce deformation or fracture. Thin features are also prone to vibration, which makes accurate machining challenging and increases machining time. 

To minimize cost:

• For metal parts, design walls thicker than 0.8 mm; thicker walls improve stability and reduce machining time. 

• For plastic parts, keep minimum wall thickness above 1.5 mm. 

Good to know: Minimum achievable wall thickness is about 0.5 mm for metals and 1.0 mm for plastics. Evaluate the machinability of these features case by case. 

Important: Thin walls often cause problems when holes or threads are placed close to an edge. Account for this during CNC design.

4. Limit the length of threads

Excessive thread length increases CNC cost by requiring special tooling and longer cycle times. Thread engagement beyond 1.5 times the hole diameter does not significantly increase joint strength. 

To minimize cost: 

• Limit thread length to a maximum of three times the hole diameter. 

• For blind holes, leave an unthreaded relief at the bottom at least half the hole diameter. 

5. Use standard hole sized

Holes can be CNC machined quickly and accurately using standard drill bits. Nonstandard sizes require an additional machining step, which increases cost. When possible, use through holes instead of blind holes because they are easier to machine. 

Limit hole depth to four times the diameter. Deeper holes, up to about 10 times the diameter, are possible but will increase cost because they require longer machining time. 

To minimize cost:

• Size holes in 0.1 mm increments up to 10 mm, and in 0.5 mm increments for diameters above 10 mm. 

• When designing in inches, use conventional fractional sizes or reference a fractional drill bit size table. 

Using standard thread sizes in your CNC designs helps reduce lead time. This shortens machining time and lowers overall cost. 

6. Only specify tolerances when necessary

Tight tolerances increase machining cost and should be applied only when required. If a specific tolerance is not defined on the technical drawing, parts are machined to the standard tolerance (±0.125 mm or better), which is sufficient for most noncritical features. 

To minimize cost:

• Specify tighter tolerances only when necessary. 

• Use a single datum, for example the intersection of two edges, as the reference for all toleranced dimensions. 

Pro tip: Use geometric dimensioning and tolerancing (GD&T) on technical drawings to reduce CNC machining costs. GD&T controls features such as flatness, straightness, circularity, and true position. It often allows looser size tolerances while meeting function, but it requires advanced design knowledge to apply effectively. 

7. Minimize the number of machine setups

Design parts to be machined in as few setups as possible, ideally a single setup. For example, a part with blind holes on both faces requires two setups because it must be rotated to access each side. 

Rotating or repositioning a part increases manufacturing cost because it is often a manual step. Complex geometries may require custom fixturing, which adds expense. Highly complex shapes may need a multi-axis CNC system, further increasing cost. 

Consider splitting the design into multiple components that can each be CNC machined in a single setup and then bolted or welded together. This approach also helps for parts with very deep pockets. 

To minimize cost:

• Design parts with simple 2.5D geometry that can be manufactured in a single setup. 

• If that is not feasible, split the design into multiple components that can be assembled afterward. 

8. Avoid small features with high aspect ratio

Small, slender features with a high width-to-height ratio are prone to vibration, making precise machining difficult. 

To minimize cost:

• Keep feature width-to-height aspect ratio below 4:1. 

• Add bracing around small features or connect them to a wall to increase stiffness. 

9. Remove all text and lettering

Adding text to a CNC machined part can significantly increase cost because it requires additional toolpaths and machining time. Surface finishing methods such as silk screening or painting are more cost effective for adding text to CNC machined parts. 

To minimize cost:

• Remove all text and lettering from CNC machined parts. 

• If text is required, choose engraved rather than embossed lettering. 

• Use a minimum size 20 sans serif font, such as Arial or Verdana. 

10. Consider the machinability of the material

Machinability refers to the ease with which a material can be cut. The higher the machinability, the faster a material can be CNC machined, thereby lowering cost. Machinability depends on the physical properties of each material. Typically, the softer and more ductile a metal alloy, the easier it is to machine. 

C360 brass is the alloy with the highest machinability, allowing for high speed machining. Aluminum alloys (e.g. 6061 and 7075) can also be machined very easily, though require slightly lower speeds. 

Stainless steel has 10 times lower machinability than aluminum and will take at least twice as much time to machine. Different steel grades have different machinability. For example, 304 stainless steel has a machinability index of 45 percent, while 303 stainless steel (an alloy with very similar chemical composition) has an index of 78 percent, making it easier to machine.

The machinability of plastics mainly depends on their thermal properties and stiffness because they are prone to melting and bending during machining. 

POM (Derlin) is the easiest plastic to machine, while ABS comes in a close second. PEEK and nylon 6 are common engineering plastics that are more difficult to machine.

To minimize cost:

• When possible, choose a material with higher machinability, especially for larger production runs. 

11. Consider the price of the bulk material

The cost of bulk material is another factor that can significantly affect the price of CNC machined parts. The table below summarizes the prices of common metal alloys and plastics used in CNC for a 6 in x 6 in x 1 in sheet (approximately 150 x 150 x 25 mm). 

Source: McMaster

Aluminum 6061 is one of the most cost-effective choices for metal prototypes thanks to its low material cost and excellent machinability. 

Metals with higher machinability, such as stainless steel 303 and C360 brass, generally cost more and are better suited to larger production runs. At scale, economies of scale apply because faster cycle times and shorter machining offset the higher material cost. 

For plastics, ABS, nylon, and POM (Delrin) are priced similarly to aluminum 6061, but they are more difficult to machine, which can increase overall cost. PEEK is a high cost material and should be specified only when its performance is essential. 

To minimize cost: 

• Choose a material with a low raw material cost, especially for low-volume orders. 

12. Avoid multiple surface finishes

Surface finishes improve the appearance and environmental resistance of CNC machined parts, but they add cost. Specifying multiple finishes on the same part increases cost further because it requires extra steps, such as masking. For a summary of finish options and benefits, see our article on CNC surface finishes. 

To minimize cost:

• Choose the standard “as machined” surface finish where possible. 

• Request multiple surface finishes only when necessary. 

13. Account for blank size

Blank size affects overall cost. As a rule of thumb, select stock that is at least 3 mm larger than the finished part in all dimensions. This allows material to be removed from every edge to achieve final size and accuracy. 

For example, if a part has an envelope of 30 x 30 x 30 mm, it typically requires a larger blank cut from a 35 mm sheet. If the envelope is reduced to 27 x 27 x 27 mm, a 30 mm sheet can be used instead, which saves material and lowers cost. 

To minimize cost:

• Design parts to be at least 3 mm smaller than the nearest standard blank size. 

14. Take advantage of economies of scale

In CNC machining, order quantity strongly influences unit price. Start-up costs are relatively high, so at low volumes they make up a large share of the cost per part. As volume increases, these fixed costs are spread across more parts, reducing the unit cost. 

In the graph below, we show the average unit price for 12 parts machined in 304 stainless steel.  

The unit price drops nearly exponentially: increasing quantity from one to five can cut the price by about half, and ordering very high volumes (over 1,000 parts) can reduce unit cost by five to ten times. 

To minimize cost:

• Leverage economies of scale by ordering higher volumes. 

Best practices for lowering CNC costs

In conclusion, keep your CNC machining simple. 

Complexity increases cost. Designs that require special tooling or fixtures, multiple machine setups, or specialty materials drive higher pricing. 

To reduce CNC machining cost, review these questions before requesting a quote: 

• Is my part designed using design for machinability (DFM) guidelines? 

• Are all features essential, or can I remove or simplify them while maintaining full functionality? 

• Can the design be split into multiple parts that are easier to machine and assemble later? 

• Can I modify the design to avoid multiple machine setups or special tooling? 

• Is there a lower cost or more machinable material that still meets my design requirements? 

The present & the future of CNC machining

CNC machining capabilities continue to expand. Recent advances in tooling allow modern systems to thread holes along their full length, and holes of virtually any diameter can be produced with minimal impact on price by using a plunging tool and profile interpolation, such as a helical tool path. 

This article covers design for manufacturability tips that apply to any CNC system. Treat these as practical guidelines to help you design parts more efficiently and ready for production. 

Download the CNC checklist for reducing costs

If you found this article useful and want an offline reference, download our CNC machining cost reduction checklist.