Are you machining your threaded holes correctly? Is the machining efficient?
Are you still struggling with poor threaded hole machining?
Have you thought about how you can optimize the way you machine threaded holes.
I am the Chief Technical Expert at Santanoo Technology, with 15 years of experience in CNC machining across China and Japan.
My team and I have solved numerous CNC machining issues for over 600 clients in various industries.
To help you make informed decisions about the methods to use for machining threaded holes, increase production efficiency, reduce costs, and avoid quality defects, we'd like to share some insights.
What Are Threaded Holes and Why Important?
Threaded holes are spiral-shaped geometrical features composed of external ridges and internal grooves. Due to their efficient fastening capabilities, they are widely used in industrial and construction fields. Applications range from automobiles and machinery to structural assemblies.
Advantages of threaded holes include controlled tightening force, compact connection structure, high reliability, and resistance to loosening.
Evolution of Threaded Hole Machining Methods
With improvements in CNC machining center capabilities and cutting tool technologies, threaded hole machining methods are continuously evolving, leading to increased precision and efficiency.
The common methods used in CNC machining centers for threaded hole production are primarily:
- Tap Machining
- Thread Milling
1. Tap Machining
This is the most commonly used method for machining threaded holes, especially those with smaller diameters (D<30) and less stringent positional accuracy requirements.
1.1 Types and Characteristics of Tap Machining
There are two main types of tap machining:
- Flex Tapping: Utilizes a flexible tap holder, which allows axial compensation, thereby reducing the feed error caused by the non-synchronization of spindle feed and rotation, ensuring correct thread pitch.
- Rigid Tapping: Employs a rigid spring clamp to hold the tap, where both the feed and rotation of the spindle are controlled by the machine. With the improved performance of CNC machining centers, rigid tapping has become the standard configuration and primary method for threaded hole production.
Comparison:
| Aspect | Flex Tapping | Rigid Tapping |
|---|---|---|
| Clamp Structure | Complex | Simple |
| Cost | High, easily damaged | Low, durable |
| Efficiency | Low-speed cutting, lower efficiency, no re-tapping | High-speed cutting, higher efficiency, allows re-tapping |
1.2 How to Achieve High-Precision Threaded Holes with Tap Machining
- Center Drilling for Positioning
- Drill the Pilot Hole
- Tap Machining
1.2.1 Selection of Drills
The selection of the right drill has a significant impact on the tap's life and the quality of the threaded hole. For instance, for an M8 threaded hole with a pilot hole diameter of Ф6.7±0.27 mm, a Ф6.9 mm drill is ideal for reducing the machining allowance and extending the life of the tap.
1.2.2 Selection of Taps
When choosing the correct tap, consider:
- Material of the Workpiece: Different taps are designed for different materials. Using the wrong type can result in thread chipping or even breaking of the tap.
- Type of Hole (Through or Blind): Depending on whether the hole is through or blind, different taps like straight-flute, spiral-flute, or point-taps should be chosen.
2. Thread Milling
Thread milling is a method used for machining threaded holes in larger diameters and hard-to-machine materials. It involves the simultaneous movement of three axes: X, Y for circular interpolation and Z for linear feed.
2.1 Characteristics of Thread Milling
- High speed, efficiency, and precision: Cutting tools are usually made of carbide, capable of high-speed movement.
- Versatility: The same cutting tool can be used for both left-hand and right-hand threads, reducing tooling costs.
- Improved Chip Removal and Cooling: Especially useful for threading in materials like aluminum, copper, and stainless steel.
- Applicability to Short Blind Holes: Thread milling doesn’t require front-end guidance, making it suitable for machining short blind holes and holes without a chip groove.
2.2 Classification of Thread Milling Tools
Thread milling tools can be categorized as:
- Insert-Type Carbide Milling Cutters
- Solid Carbide Milling Cutters
2.3 Thread Milling CNC Programming
Thread milling tool programming is different from other tools. Incorrect programming can lead to tool damage or errors in thread machining. Below are some points to consider while programming:
- Preparation of Thread Bottom Hole: For small diameter holes, drilling should be performed. For larger holes, boring is the recommended process to ensure the accuracy of the bottom hole for threading.
- Tool Entry and Exit: Utilize an arc trajectory for tool entry and exit, typically 1/2 circle for both. Meanwhile, the Z-axis should advance 1/2 pitch to ensure the thread shape. Radius compensation should be active at this point.
- Arc Interpolation: On the X and Y axes, complete one full circle while the spindle should move one pitch length along the Z-axis to avoid thread mismatch.
- Example: To machine an M48×1.5 thread hole with a depth of 14, using a Φ16 thread milling cutter, the specific processing program would be as follows:
G0 G90 G54 X0 Y0
G0 Z10 M3 S1400 M8
G0 Z-14.75 (Move to the deepest part of the thread)
G01 G41 X-16 Y0 F2000 (Move to tool entry position, add radius compensation)
G03 X24 Y0 Z-14 I20 J0 F500 (Use a 1/2 circle arc for entry)
G03 X24 Y0 Z0 I-24 J0 F400 (Machine the entire thread)
G03 X-16 Y0 Z0.75 I-20 J0 F500 (Use a 1/2 circle arc for exit)
G01 G40 X0 Y0 (Return to center, cancel radius compensation)
G0 Z100 M30
