Creating internal threads is a fundamental operation in manufacturing, but it’s also one of the most high-stakes processes a machinist can perform. On a manual machine, the operator can “feel” the cut. On a CNC mill, the process is blind, trusting the machine’s precision. A broken tap can turn a high-value part into scrap in seconds.
However, modern CNC mill tapping is incredibly reliable when you understand the principles, select the right tools, and use the correct programming. This guide provides a comprehensive overview of how to tap holes perfectly on your CNC milling machine, from tooling and programming to troubleshooting.

The Two Core Tapping Methods: Rigid vs. Floating

The first major decision is how the machine will synchronize the tool’s rotation and feed. This choice depends entirely on your machine’s capabilities.

1. Rigid Tapping

Rigid tapping is the modern standard and the preferred method on nearly all new CNC mills.

• How it works: The machine’s control perfectly synchronizes the spindle’s rotation (RPM) with the Z-axis feed rate ($F$). The spindle knows its exact angular position and advances the tap precisely one pitch per revolution.
• Tooling: It requires a solid, high-quality tool holder, such as a high-precision ER collet chuck or a dedicated rigid tapping holder. There is no “play” or flexibility.
• Pros:
  ◦ Extremely accurate thread depth.
  ◦ Faster cycle times.
  ◦ Better thread quality.
  ◦ Simpler and more reliable programming.

1. Floating Tapping (Tension-Compression)

This method is used on older CNC machines that do not have a synchronized spindle.

• How it works: It uses a special “floating” tap holder, often called a tension-compression holder. This holder has a built-in mechanism that allows the tap to “float” or travel slightly along the Z-axis, independent of the machine’s feed. This small amount of tension (pulling) and compression (pushing) compensates for any minor synchronization errors between the spindle and the feed.
• Tooling: Requires a tension-compression holder.
• Pros:
  ◦ Forgiving on machines without true rigid tapping.
• Cons:
  ◦ Slower, as the machine must decelerate/accelerate more carefully.
  ◦ Less precise control over thread depth.
  ◦ Holders are more complex and expensive.
  The Verdict: If your machine supports it (and most machines from the last 20 years do), always use rigid tapping.

Choosing Your Tool: Cut Taps vs. Form Taps

Not all taps are created equal. The most significant division is between taps that cut material and taps that form it.

Cut Taps (Chip-Forming Taps)

As the name implies, these tools have cutting edges that shear the material to create the thread profile, producing chips just like a drill or end mill.

• Spiral Point Taps (Gun Taps): These taps have a straight flute with an angled “point” at the tip. This point is designed to push the chips forward and out of the way.
  ◦ Best Use: Through-holes, where chips can fall freely out the bottom.
• Spiral Flute Taps: These look more like a standard drill bit, with helical flutes. The helix acts like an auger, pulling the chips backward and out of the hole.
  ◦ Best Use: Blind holes, where chips cannot go forward. Using a spiral point tap in a blind hole is a primary cause of tap breakage.
• Straight Flute Taps: These are the most basic type, often used for hand tapping. They are generally not recommended for high-performance CNC work as they offer poor chip evacuation.

Form Taps (Roll Taps / Chipless Taps)

Form taps are a game-changer for the right applications. They have no cutting edges or flutes. Instead, they displace and cold-form the material to create the thread shape.

• How it works: The tap “squeezes” the material in the pre-drilled hole, forcing it to flow into the tap’s “valleys,” thus forming the thread “peaks.”
• Pros:
  ◦ No Chips: This is the single biggest advantage. No chip management, no clogging, no re-cutting.
  ◦ Stronger Threads: The cold-working process (work hardening) makes the threads significantly stronger than cut threads.
  ◦ Longer Tool Life: With no sharp edges to dull, form taps often last 5 to 20 times longer than cut taps.
  ◦ Faster Speeds: They can often be run much faster than cut taps.
• Cons:
  ◦ Material Dependent: Only suitable for ductile materials that can be formed without cracking. This includes aluminum, most stainless steels (like 304, 316), copper, brass, and low-carbon steels. Never use them in cast iron or high-carbon (tool) steels.
  ◦ Different Drill Size: They require a larger pre-drilled hole than a cut tap, as material is displaced, not removed.
  ◦ Higher Torque: The forming process requires more spindle torque.
  The Verdict: For through-holes, use a spiral point tap. For blind holes, use a spiral flute tap. For high-volume production in ductile materials, form tapping is the clear winner.

The Step-by-Step Tapping Process

Follow these steps for a successful tapping operation every time.

Step 1: Hole Preparation (The Most Critical Step)

You cannot create a good thread from a bad hole.

1. Drill the Correct Size: This is non-negotiable. Look up the correct tap drill size for your thread (e.g., “M8x1.25 tap drill”). Crucially, the drill size is different for cut taps vs. form taps. A form tap drill chart will show a much larger diameter.
2. Ensure Hole Quality: The hole should be round, straight, and on-location.
3. Chamfer the Hole: Always add a small chamfer (countersink) to the top of the hole. This:
   ◦ Helps guide the tap and prevents it from “walking.”
   ◦ Removes the sharp burr.
   ◦ Creates a clean, professional lead-in for the fastener.
   The chamfer diameter should be slightly larger than the tap’s major diameter.

Step 2: Tool Setup

• Holder: Use a high-quality, rigid holder for rigid tapping.
• Runout: Ensure the tap is running true with minimal runout (wobble). Any wobble will cut an oversized thread and dramatically reduce tool life.
• Probing: Use a tool probe to set the precise length of your tap. Accurate depth is key, especially in blind holes.

Step 3: Programming the Tapping Cycle

Most CNC controls use a canned cycle for tapping. The most common is G84 (Right-Hand Tapping Cycle). A typical line of G-code looks like this:
G90 G54 G00 X1.0 Y1.0 S1000 M03;
G43 H01 Z1.0 M08;
G84 Z-0.5 R0.1 F50.0;
G80;
Let’s break down the G84 line:

• G84: Activates the rigid tapping cycle.
• Z-0.5: The final thread depth.
• R0.1: The “Retract” or “Reference” plane. The tool will rapid to this height, then feed from this height to the Z depth.
• F50.0: The Feed Rate. This is the most important value in the line.
• G80: Canned Cycle Cancel.

The Golden Rule: Calculating Feed Rate

In rigid tapping, the feed rate is mathematically locked to the spindle speed. You cannot guess.
The Formula (Metric):
Feed Rate (mm/min) = Spindle Speed (RPM) × Pitch (mm)

• Example: Tapping an M6 x 1.0 thread (1.0mm pitch) at 1500 RPM.
• Calculation: Feed Rate = 1500 × 1.0 = 1500 mm/min.
• Your Code: S1500 F1500.0
  The Formula (Imperial):
  Feed Rate (in/min) = Spindle Speed (RPM) × Pitch (in)
  (Note: Pitch in inches = 1 / TPI)
• Example: Tapping a 1/4″-20 thread (20 threads per inch) at 1000 RPM.
• Pitch: 1 / 20 = 0.05″
• Calculation: Feed Rate = 1000 × 0.05 = 50 in/min.
• Your Code: S1000 F50.0
  This relationship is absolute. If you change the speed, you must change the feed. This is a core concept of CNC programming.

Step 4: Speeds and Coolant

• Speeds (RPM): The correct spindle speed depends on the tap material (HSS, Carbide), tap coating (TiN, TiAlN), and workpiece material. Always start with the tap manufacturer’s recommendations. You can find excellent technical data from sources like Sandvik Coromant’s cutting data charts.
• Coolant: Tapping generates significant heat and friction.
  ◦ Flood Coolant: For most applications, a high-quality, water-soluble flood coolant is essential for chip evacuation and lubrication.
  ◦ MQL / Tapping Fluid: For form tapping or in some hard materials, a specialized, high-lubricity cutting oil (applied via MQL or as a paste) can provide better results than standard flood coolant.

An Alternative: Thread Milling

It’s important to know that tapping is not the only way to make a thread on a mill. Thread milling is an excellent alternative.
This process uses a smaller “thread mill” tool and a helical interpolation path (G02 or G03) to “cut” the thread in multiple passes.

• Pros:
  ◦ Safer: The tool is smaller than the hole, so if it breaks, it’s easily removed.
  ◦ Versatile: One tool can cut any diameter of thread (as long as the pitch is the same).
  ◦ Control: Full control over thread fit (percent of thread) by adjusting the tool’s path.
  ◦ No Left-Hand Taps: Can cut right-hand or left-hand threads with the same tool.
• Cons:
  ◦ Slower Cycle Time: Takes longer than a single G84 cycle.
  ◦ More Complex Programming: Requires helical interpolation.
  Thread milling is ideal for large, expensive parts where a broken tap would be a catastrophe, or for non-standard thread diameters.

Troubleshooting Common CNC Tapping Problems

Even with perfect programming, issues can arise. Here’s what to look for.

• Problem: Tap Breakage
  ◦ Cause 1 (Chip Clogging): You’re using a spiral point (gun) tap in a blind hole. Fix: Switch to a spiral flute tap.
  ◦ Cause 2 (Wrong Drill Size): The tap drill hole is too small. Fix: Verify your drill size. Remember form taps need a larger hole.
  ◦ Cause 3 (Dull Tap): The tap is worn out. Fix: Replace the tap.
  ◦ Cause 4 (Misalignment): The tap is not entering the hole straight. Fix: Check tool runout.
• Problem: Oversized or Galled Threads
  ◦ Cause 1 (Material): You are form tapping a “gummy” material (like 304 Stainless or some aluminums) and it’s “pushing” instead of shearing. Fix: Use a high-lubricity cutting fluid (not just coolant) or switch to a cut tap.
  ◦ Cause 2 (Speed): Your RPM is too high, generating too much heat. Fix: Reduce spindle speed.
  ◦ Cause 3 (Dull Tap): A worn-out tap will “smear” the material. Fix: Replace the tap.
• Problem: Poor Thread Finish
  ◦ Cause 1 (Speed): RPM is often too fast or too slow. Fix: Adjust speed based on manufacturer data.
  ◦ Cause 2 (Coolant): Ineffective coolant. Fix: Check concentration and flow.
  ◦ Cause 3 (Wrong Tap): Using the wrong tap geometry for the material. Fix: Consult a tooling expert. More info can often be found from manufacturing authorities like the Society of Manufacturing Engineers (SME).

Conclusion: Tapping with Confidence

CNC mill tapping has evolved from a high-risk operation to a reliable and precise process. By investing in high-quality CNC machines with robust rigid tapping capabilities, you eliminate many historical variables.
The keys to success are:

1. Prepare the hole correctly (drill size and chamfer).
2. Choose the right tool (rigid vs. floating, cut vs. form).
3. Obey the Golden Rule: Feed = RPM × Pitch.
   By following these guidelines, you can program tapping cycles with confidence and produce perfect threads every time.

Disclaimer

The information provided in this article is for informational purposes only. The practical application of this information involves significant risks of equipment damage and personal injury. All CNC programming and machining operations should be performed or supervised by qualified professionals. Always consult your machine’s manuals, tooling manufacturer’s specifications, and follow all established safety protocols. XproCNC and the author assume no liability for any damages or injuries resulting from the use or misuse of this information.