What is Tap drill Size?

“Tap Dill Size” is the drill diameter we should use before a tapping operation. By default, the size you will find on most charts is the diameter for 75% thread depth on a Cutting Tap. Here you will learn how to get the right drill diameter depending on the tap type and required thread height.

## Tap Drill Size Formulas

Parameters:

• TD – Tap Drill Diameter (mm / Inch)
• D – Nominal Thread Diameter (mm / Inch)
• H – Thread Depth (mm / Inch)
• Hp – Thread Depth (In percentage)
• Hp = 100*(Hmax-H)/Hmax
• PPitch (distance in mm)
• TPI – Pitch (Pitch expressed as tooth per Inch)

Formulas:

Tap Cutting

$$\LARGE D - \frac{H_p}{76.98\,\times\,TPI}$$
$$\LARGE D - \frac{H_p\,\times\,P}{76.98}$$
Tap Forming

$$\LARGE D - \frac{H_p\,\times\,P}{294.12}$$
$$\LARGE D - \frac{H_p}{294.12\,\times\,TPI}$$

## Thread Depth (Height) in tapping Explained

The distance between the crest and root is called the thread height. The thread standards define the maximum thread height and are the same for metric and inch threads.

$$H_{max}=\Large \frac{5}{8}\times\frac{\sqrt{3}}{2}\normalsize\times{P}\,=\,0.5413\times{P}$$
$$H_{max}=\Large \frac{5}{8}\times\frac{\sqrt{3}}{2}\normalsize\times{P}$$ $$\,=\,0.5413\times{P}$$

In tapping, it is customary to express the thread height (Sometimes called thread depth) as the relation in percentage between the actual depth and the maximum depth.

$$H_{p}=\Large \frac{H_{max}\,-\,H}{H_{max}}\normalsize\times{100}$$
• A larger Thread height means a smaller tap drill size.
• A smaller Thread height means a larger tap drill size.

Why Is it important?

• Since the feed always equals the thread pitch and the entire thread depth is machined in one pass by definition, these factors are not in our control. The thread depth is a primary factor (Next to the cutting speed) influencing a tapping tool’s torque and tool life.
• Increasing the drill size makes tapping easier and extends the tool-life of the tap. However, the strength of the thread is reduced, and the minor diameter can get out of tolerance.
• It is an informal rule that the default thread depth is 75%. Therefore, in most charts you will find in various catalogs or on the web, the value given for the tap drill size is 75% thread height. The actual working range in most cases is 65%-85%.

With our Calculator  and Chart , you can get the precise tap drill size as a function of the thread height.

## Calculation Examples

Calculating Tap Drill Size for M8 X 1.25 (Metric Thread)

$$\begin{array}{l} D=8\text{ mm} \\ P=1.25\text{ mm} \\ H_p=65\text{%} \\ TD = 8\,-\,\Large \frac{65\,\times\,1.25}{76.98}\normalsize=\,6.94\text{ mm} \end{array}$$

Calculating Tap Drill Size for UNC 1/4-20 (InchThread)

$$\begin{array}{l} D=0.25\text{“} \\ TPI=20\text{ Tooth per Inch} \\ H_p=80\text{%} \\ TD = 0.25\,-\,\Large \frac{80}{76.98\,\times\,20}\normalsize=\,0.198\text{“} \end{array}$$
• The above examples are for cutting taps.

## Tapping technologies

### Cutting Taps

• The cutting taps are far more popular and can be used on all materials.
• As its name suggests, it cuts the material in the same way as a milling or turning tool by removing material and generating chips.
• They have flutes (Usually straight).
• The bore diameter created by the tap drill does not change and is the minor diameter of the thread.

### Forming Taps

• The forming taps are an alternative solution for cutting taps when machining a thread in soft materials such as aluminum, brass, copper, 300 stainless steel, and low carbon steel.
• As its name suggests, it forms the thread by pressing the material.
• They Don’t have flutes (Sometimes they have narrow lubrication grooves).
• The bore diameter created by the tap drill gets smaller due to the material that is pushed to create a thread. This “material growth” should be taken into account.

Advantages of Forming Taps (Compared with cutting taps):

• The cycle time is shorter due to higher cutting speeds.
• Better uniformity and accuracy of the thread.
• A higher strength of the thread (Due to internal stress created by the forming process).
• No chips are formed, therefore there is never a chip evacuation issue.

Disadvantages of Forming Taps (Compared with cutting taps):

• They can be used only on ductile materials such as aluminum, brass, copper, 300 series stainless steel, and low carbon steel
• Forming taps generate higher torque. This becomes more problematic in larger diameters.
• They are more sensitive to fractures, especially if not applied correctly.

## Tap Dill Size Chart

### Unified Inch Threads (UNC/UNF/UNEF) Tap Drill Size Chart

Tap Drill size per thread height (In percentage)

• Press to view all Width (55%-85%).

### Metric Threads Tap Drill Size Chart

Tap Drill size per thread height (In percentage)

• Press to view all Width (55%-85%).
Scroll to Top