Threading operations are among the most common features we machine at Anco Precision. Whether you're designing a prototype housing with tapped mounting holes or a production run of threaded fittings, understanding how thread design affects machining cost and lead time helps you get better quotes and avoid manufacturing issues.
This article covers practical considerations for CNC machined threads from a machine shop perspective, including thread depth requirements, hole configurations, standard thread sizes, and the drawing information that helps us provide accurate quotes quickly.
Thread Depth Considerations
Thread depth directly affects tool selection, cycle time, and part cost. The depth you specify should balance functional requirements with manufacturing efficiency.
Minimum Thread Depth
For most applications, a thread depth of 1.5 times the nominal diameter provides full thread strength. A 1/4-20 thread, for example, needs approximately 0.375 inches of engaged thread depth to develop the full strength of the fastener. Specifying more depth than necessary increases machining time without adding functional value.
When space permits, we typically recommend 1.5 to 2 times the diameter for tapped holes. This provides adequate engagement while leaving room for tap runout at the bottom of blind holes.
Maximum Practical Depth
Deep threaded holes present challenges. Chip evacuation becomes difficult, tap breakage risk increases, and cycle times grow. As a general guideline, thread depths beyond 2.5 to 3 times the diameter require careful consideration.
If your design requires deep threads, consider whether a through hole is possible, whether the hole can be drilled from both sides, or whether a helical insert might provide a better solution. These alternatives often reduce cost and improve reliability.
Blind Holes Versus Through Holes
The choice between blind and through holes significantly impacts machining operations and cost.
Through Holes
Through holes are generally easier and faster to machine. Chips evacuate freely, taps don't need to stop at a precise depth, and there's no concern about tap runout at the bottom of the hole. When your design allows it, through holes typically cost less and have shorter lead times.
If the through hole will be visible or if you need to prevent fluid passage, consider whether a set screw, plug, or O-ring seal can address the requirement while maintaining the manufacturing advantages of a through hole.
Blind Holes
Blind threaded holes require additional considerations. The hole must be drilled deeper than the required thread depth to accommodate tap runout—the unthreaded portion at the bottom where the tap tapers. Typically, we add 2 to 3 thread pitches beyond the required thread depth for tap clearance.
For example, a 1/4-20 blind hole with 0.375 inches of required thread depth needs a total drilled depth of approximately 0.475 to 0.525 inches. This clearance prevents the tap from bottoming out and potentially breaking.
Blind holes also require peck drilling cycles to clear chips and may need compressed air or coolant to ensure complete chip evacuation. These factors add cycle time compared to through holes.
Standard Thread Sizes
Using standard thread sizes reduces cost and improves availability. Standard taps are readily available, less expensive, and familiar to machinists.
Unified National Coarse and Fine Threads
In the United States, UNC (coarse) and UNF (fine) threads are the most common standards. Examples include 1/4-20 (coarse), 1/4-28 (fine), 10-24 (coarse), and 10-32 (fine). These threads are widely used in mechanical assemblies and hardware.
Coarse threads are generally easier to machine, more forgiving of minor damage, and easier to assemble. Fine threads provide finer adjustment and better vibration resistance but are more susceptible to cross-threading and damage.
Metric Threads
Metric threads follow ISO standards with designations like M6x1.0 or M8x1.25. The first number indicates the nominal diameter in millimeters, and the second indicates the pitch in millimeters. Coarse metric threads often omit the pitch designation (M6 implies M6x1.0).
When designing parts with metric threads, verify that you're specifying standard pitches. Non-standard metric threads require special taps that may have longer lead times and higher costs.
Pipe Threads
NPT (National Pipe Taper) and NPTF (National Pipe Taper Fuel) threads are tapered threads used primarily for pressure-tight joints in fluid systems. These threads require different machining approaches than straight threads and have specific depth and tolerance requirements.
If your application requires pipe threads, clearly specify whether you need NPT, NPTF, or straight pipe threads (NPS). The distinction affects both machining and assembly.
Special and Custom Threads
Non-standard threads—whether custom pitches, unusual diameters, or proprietary thread forms—require special tooling. This increases both cost and lead time. If your design requires a non-standard thread, be prepared for these additional expenses and provide complete thread specifications including pitch, depth, tolerance class, and any relevant standards.
Drawing Information for Accurate Quotes
The quality and completeness of your drawing or CAD file directly affects how quickly we can quote your project and how accurately we can machine your parts. The drawing typically serves as the controlling specification for the machined part.
Thread Callouts
Thread callouts should include the thread size, pitch or threads per inch, thread class or tolerance, and depth. A complete callout might read "1/4-20 UNC-2B x 0.50 DEEP" for a blind hole or "M8x1.25-6H THRU" for a metric through hole.
The thread class (2B for internal inch threads, 6H for internal metric threads) indicates the tolerance. Class 2B and 6H are standard fits suitable for most applications. If you need a tighter or looser fit, specify it clearly.
Hole Location and Orientation
Dimension threaded holes from established datums using coordinate dimensions or geometric dimensioning and tolerancing. If hole location is critical for assembly, specify the positional tolerance.
For angled or compound-angle holes, provide clear views or section views showing the hole orientation. Ambiguous drawings lead to clarification delays or manufacturing errors.
Material Specification
Material selection affects thread strength, machinability, and tool life. Common materials for threaded parts include aluminum alloys (6061-T6, 7075-T6), stainless steels (303, 304, 316), carbon steels, brass, and engineering plastics.
Some materials machine threads more easily than others. Aluminum and brass cut cleanly with standard taps. Stainless steel is more challenging and may require specialized taps or thread milling. If material selection is flexible, mention that in your RFQ—we may be able to suggest alternatives that reduce cost or lead time.
Quantity Requirements
Quantity affects our quoting approach. Small quantities may use different setups or processes than large production runs. Be clear about your immediate quantity needs and potential future volumes.
If you're ordering prototype parts with the possibility of production orders later, mention that. It helps us understand your project timeline and may influence our recommendations for design optimization or process selection.
Tolerances and Critical Features
General tolerances typically apply to most features, but threaded holes often have specific requirements. If thread depth, hole location, or perpendicularity is critical, call it out explicitly.
Standard thread tolerances (2B for inch, 6H for metric) are appropriate for most applications. Tighter tolerances require additional operations or inspection and increase cost.
Surface Finish Requirements
Threaded holes typically don't require special surface finish callouts—the tapping operation produces a functional finish. If you need a specific finish on other part surfaces, specify it clearly using Ra values or finish symbols.
Inspection and Documentation
If your project requires specific inspection documentation, dimensional reports, material certifications, or compliance with particular standards, include that information in your RFQ. Some customers need detailed inspection reports or certifications for aerospace, medical, or other regulated applications. Knowing these requirements upfront helps us provide accurate quotes and lead times.
Prototype Versus Production Considerations
The approach to threading operations may differ between prototype and production work, though both typically use CNC equipment at our shop.
For smaller quantities, we evaluate the most efficient setup for your specific parts. This might involve tapping operations in the CNC machining center, secondary tapping operations, or thread milling depending on the thread size, material, and part geometry.
For larger production runs, we optimize the process for cycle time and tool life. This might include dedicated tapping fixtures, coolant-through tooling, or thread milling for difficult materials. The setup time is amortized over more parts, making these optimizations cost-effective.
If you're starting with a prototype and anticipate production orders, let us know. We can design the initial setup with future production in mind, potentially reducing costs when you scale up.
RFQ Checklist for Threaded Parts
When requesting a quote for parts with CNC machined threads, include the following information:
- Engineering drawing or CAD file: Provide a PDF drawing or STEP file showing all dimensions, thread callouts, and specifications
- Material: Specify the material grade (e.g., 6061-T6 aluminum, 304 stainless steel) or indicate if alternatives are acceptable
- Quantity: State your required quantity and mention if you anticipate repeat orders
- Tolerances: Note any critical dimensions or features beyond standard tolerances
- Surface finish: Specify if you need particular surface finishes or coatings
- Required completion date: Provide your target delivery date or project timeline
- Inspection requirements: Mention if you need dimensional reports, material certs, or other documentation
- Special notes: Include any additional requirements such as marking, packaging, or assembly considerations
The more complete your RFQ, the faster we can provide an accurate quote and the less likely we'll need to request clarifications.
Common Thread Design Issues
A few thread design issues appear frequently in RFQs. Avoiding these can save time and reduce costs.
Insufficient Wall Thickness
Thin walls around threaded holes can crack during tapping or strip during assembly. As a general rule, maintain wall thickness of at least 1.5 times the thread diameter when possible. For smaller threads in strong materials, you may get away with less, but it's worth evaluating.
Threads Too Close to Edges or Features
Threads located very close to part edges, pockets, or other features can be difficult to machine and may compromise part strength. Leave adequate material around threaded holes—typically at least one thread diameter from edges when possible.
Unclear Thread Specifications
Incomplete thread callouts lead to clarification requests and delays. Always specify thread size, pitch or TPI, thread class, and depth. If you're using a non-standard thread, provide complete specifications or a detail drawing.
Unnecessarily Tight Tolerances
Standard thread classes (2B for inch, 6H for metric) work for most applications. Specifying tighter tolerances without functional justification increases cost. If you need a precision fit, specify it clearly, but avoid over-tolerancing.
Request a Quote for Your Threaded Parts
At Anco Precision, we machine threaded parts daily in a wide range of materials and configurations. Whether you need a few prototype parts with tapped holes or a production run of threaded components, we can help.
To request a quote, send us your drawing or STEP file, material specification, quantity, any critical tolerances or requirements, and your required delivery date. We'll review your project and provide a detailed quote.
If you have questions about thread design, material selection, or manufacturing approach, we're happy to discuss your project. Contact Anco Precision today to get started on your next machining project.