Free Tap Speed and Feed Calculator
Pick the thread and the workpiece material, and the calculator gives you the tapping speed (RPM), the tapping feed rate, and the tap drill size for a 75% thread. It handles UNC/UNF and ISO metric threads, and writes the G84 rigid tapping line for you.
Tap Speed and Feed Calculator
Rigid tapping: G84 Z-0.500 R0.100 F30.6 S611
For cutting taps in HSS. Speeds are the middle of the ranges in the table below; edit the surface speed to override it. RPM = SFM × 12 ÷ (π × tap diameter); feed rate = RPM ÷ TPI (or RPM × pitch in mm). The G84 line assumes feed per minute (G94); set the depths for your part.
Tap Feeds and Speeds Basics
Tapping Feeds and Speeds are pretty easy to calculate because they're constrained by the thread that is being tapped. Everything starts from Tapping Speeds
What Tapping RPM or Tapping Speed Should I Use?
The spindle speed depends upon the material you're trying to tap and the diameter of the tap. The calculator above works it out from the surface speeds in this table.
Recommended Surface Speeds (SFM) by Material
We can find the recommended surface speed to tap many workpiece materials in this table:
| Workpiece Material | Surface Speed (SFM) |
|---|---|
| Aluminum - Cast Alloys | 60 |
| Aluminum - Diecast Alloys | 70 |
| Aluminum - Wrought Alloys | 80 |
| Brass | 60-100 |
| Bronze | 30-40 |
| Copper | 60-80 |
| Gun Metal | 50-60 |
| Cast Iron - Grey | 30-60 |
| Cast Iron - Ductile | 50 |
| Cast Iron - Alloys | 15-30 |
| Malleable Alloy | 20-40 |
| Magnesium Alloys | 50-70 |
| Nickel Alloys | 10 |
| Nimonic Alloys | 10-12 |
| Mild Steel | 30-50 |
| Steel - Medium Carbon | 35 |
| Tool Steel | 15-25 |
| Cast Steel | 25 |
| Titanium Alloys | 10 |
| Stainless Steel - 300 Series | 10-20 |
| Stainless Steel - 400 Series | 15 |
| Plastic | 50-70 |
| Zinc - Diecasting | 80 |
Given SFM from the table, plus the tap's diameter, we can calculate rpm with this formula:
Spindle RPM = SFM / circumference of tap
circumference of tap = PI * tap diameter
BTW, that's from our article on RPM from Surface Speed if you want the details.
Tapping Feed Rate & Tapping Feed Rate Formula
Given the spindle rpm's the Tapping Feed Rate is just how fast we have to feed to move one full thread per spindle revolution. It's our spindle rpm divided by our threads per inch (TPI).
So if we're going 1000 rpm and cutting a 20 TPI thread, we need to advance 1000/20 = 50 IPM. That's our Tapping Feed Rate, and you couldn't hope for an easier feed calculator.
[ More Cutting Speed Formulas ]
Want to Avoid Breaking Taps?
Of course you want to avoid breaking taps. A broken tap can ruin your whole day. One of the best ways to break fewer of them is to pay attention to thread percentage. Here's the dirty little secret of tapping:
The recommended hole size for tapping is usually not the best. There is no one perfect size, but you can often do a lot better by considering the thread percentage.
The deal with thread percentage is the recommended tap drill sizes you find in most online charts and on the tap packaging are for 75% threads. That's conservative from a strength standpoint, but aggressive from the standpoint of over-stressing your tap. Premium tap makers like Guhring actually recommend 60% to 70% percentage of thread for most applications because it significantly lowers the torque force required to tap without giving up much thread strength. That means you're way less likely to break the tap and you're sacrificing very little holding strength. You get much better tool life by slightly lower percentage of thread.
You can learn a bunch more from our article on tap drill sizes, but now you know enough to greatly reduce your chances of breaking a tap. It's impossible to optimize tool life without considering the thread percentage and by using proper tapping speeds. Your cutting tool will thank you if you do both.
Need to Program Tapping on a CNC?
We've got you covered with this great article on tapping G-code. It even includes information on our easy Conversational CNC Wizard for tapping.
More Feeds and Speeds Calculators
- Milling Speeds and Feeds Calculator
- CNC Router Feeds and Speeds Calculator
- Lathe Feeds and Speeds Calculator
- Drilling Speeds and Feeds Calculator
- Tap Speed and Feed Calculator
- Chip Load Calculator
- SFM to RPM Calculator
- All free CNC calculators
Be the first to know about updates at CNC Cookbook
Join our newsletter to get updates on what's next at CNC Cookbook.