Thread Mill Technical Support
Welcome to the Scientific Cutting Tools Thread Mill Technical Support page. This resource is designed to help you get the most out of your thread milling operations by providing essential technical guidance and best practices. Here, you'll find a comprehensive speed and feed chart, application guidelines to optimize performance, and practical setup and calculation tips to ensure accuracy and efficiency.
To simplify programming, be sure to use our Thread Mill Code Generator, a convenient tool that helps you create accurate G-code for your specific application. Whether you're new to thread milling or looking to refine your process, our support materials are here to assist you every step of the way. For additional support, visit our YouTube channel or check out our latest webinar on thread mills.
Speed and Feed Chart
When machining materials with an unfavorable length-to-diameter ratio, coarse thread pitches, or hard materials, you may need to use more radial depth passes than indicated on the speed and feed chart.
| Material | HB/Rc | Speed(SFM) Uncoated | Speed(SFM) AlTiN+ | Feed(Inches per Tooth) Tool Diameter .032 - .056 | Feed(Inches per Tooth) Tool Diameter .059 - .090 | Feed(Inches per Tooth) Tool Diameter .100 - .190 | Feed(Inches per Tooth) Tool Diameter .200 - .350 | Feed(Inches per Tooth) Tool Diameter .370 - .595 | Feed(Inches per Tooth) Tool Diameter .600+ |
|---|---|---|---|---|---|---|---|---|---|
| Cast Iron | 160 HB | 100-220 | 200-425 | .0004-.001 | .0004-.0008 | .0004-.0014 | .0004-.002 | .0004-.0035 | .0004-.006 |
| Carbon Steel | 18 Rc | 100-200 | 190-425 | .0003-.001 | .0003-.0008 | .0003-.0014 | .0003-.002 | .0003-.002 | .0003-.006 |
| Alloy Steel | 20 Rc | 80-200 | 200-375 | .0003-.001 2 Passes | .0003-.0008 3 Passes | .0003-.0014 | .0003-.0024 | .0003-.0024 | .0003-.006 |
| Tool Steel | 20 Rc | 80-175 | 175-250 | .0003-.0004 2 Passes | .0003-.0005 3 Passes | .0003-.0005 | .0003-.0009 | .0003-.0009 | .0003-.004 |
| 300 Stainless Steel | 150 HB | 90-120 | 120-255 | .0003-.0005 2 Passes | .0003-.0006 3 Passes | .0003-.0007 | .0003-.002 | .0003-.002 | .0003-.0045 |
| 400 Stainless Steel | 195 HB | 90-150 | 140-375 | .0003-.0005 2 Passes | .0003-.0006 3 Passes | .0003-.0007 | .0003-.002 | .0003-.002 | .0003-.0045 |
| High Temp Alloy (Ni & Co Base) | 20 Rc | 50-125 | 100-125 | .0003-.0004 3 Passes | .0003-.00045 3 Passes | .0003-.0005 2 Passes | .0003-.0009 | .0003-.0009 | .0003-.004 |
| Titanium | 25 Rc | 50-130 | 100-170 | .0003-.0004 3 Passes | .0003-.00045 3 Passes | .0003-.001 2 Passes | .0003-.0009 | .0003-.0009 | .0003-.003 |
| Heat Treated Alloys (38-45Rc) | 40 Rc | 50-90 | 90-150 | .0003-.0004 3 Passes | .0003-.00045 3 Passes | .0003-.0005 2 Passes | .0003-.0008 | .0003-.0008 | .0003-.0025 |
| Aluminum | 100 HB | 100-800 | 100-1200 | .0005-.0015 | .0005-.002 | .0005-.0025 | .0005-.003 | .0005-.003 | .0005-.009 |
| Brass, Zinc | 80 HB | 200-350 | 200-750 | .0005-.0015 | .0005-.0025 | .0005-.0025 | .0005-.003 | .0005-.003 | .0005-.009 |
Thread Cutting Pass Guidelines
When cutting threads with multiple passes, it's important to distribute the material removal evenly to balance cutting forces and improve tool life. Here's a guideline for pass distribution:
Two Passes: Cut approximately 65% of the thread on the first pass and 35% on the finish pass.
Three Passes: Use a 50/30/20 ratio for material removal.
Four Passes: Use a 40/27/20/13 ratio for optimal balance.
These ratios help to equalize the side cutting pressure, reducing tool wear and ensuring a smoother finish.
Multi-Start Threads & Thread Mills
Thread mills can be used for cutting multiple-start threads. For assistance, please contact our engineering team. Additionally, thread mills can be modified—cut off for shorter thread depths or necked back for deeper thread depths.
Adjusting Feed Rates for Internal Threads
To properly apply the Feed and Speed chart, it’s important to note that machining centers use the feed rate at the spindle’s centerline. This works for straight-line cutting, but when cutting internal threads, the feed rate must be recalculated to account for the geometry of the internal cut. Always adjust your feed rate accordingly for internal threading operations.
Speed and Feed Application
Tool Setup and Calculation Guide
Let’s do this together: we’ll walk you through the setup and calculation of cutting parameters for a TM290-24A tool used to cut a 3/8-24 thread in stainless steel.
Tool Specifications:
Tool Type: TM290-24A
Thread Size: 3/8-24
Material: Stainless Steel
Tool Outside Diameter: 0.290 inches
Chip per Tooth: 0.001 inches
Number of Flutes: 4
Calculating Revolutions per Minute (RPM):
To determine the appropriate RPM for the tool, use the following formula:
Where SFM (Surface Feet per Minute) is 150 and the tool’s outside diameter is 0.290 inches.
So, the RPM calculation is:
Calculating Non-Adjusted Feed Rate (NAFR):
Next, we calculate the Non-Adjusted Feed Rate (NAFR) using this formula:
Substituting the values:
To adjust for the major diameter of the thread, we use the following formula:
Where:
D is the major diameter of the thread (0.375 inches)
d is the tool outside diameter (0.290 inches)
Substituting the values:
The Adjusted Feed Rate (AFR) of 1.79 inches per minute ensures that the chip load per tooth remains at 0.001 inches, as specified.
Final answer to our scenario: For optimal performance, use an Adjusted Feed Rate (AFR) of 1.79 inches per minute in your CNC program. This calculation ensures precise and efficient thread cutting while maintaining the desired chip load.