Part 7 of the CNC Machining Mini-Course. Start with Part 1 if you're just joining.
---
When I first started in machining, feeds and speeds felt like black magic. Experienced machinists would dial in a number by feel, the machine would hum, chips would fly, and the part would come out beautiful. Meanwhile, I was burning up endmills and couldn't figure out why.
The truth is there is math behind it. It's not complicated math — it's algebra — but you need to understand the concepts before the formulas make sense. This post breaks it down from first principles.
---
The Two Numbers You're Solving For
Every cutting operation involves two key parameters:
Spindle Speed (RPM) — how fast the cutting tool rotates, in revolutions per minute
Feed Rate (IPM or MMPM) — how fast the tool moves through the material, in inches per minute (or mm per minute in metric)
Everything else — depth of cut, width of cut, chip load — feeds into calculating these two numbers or results from them.
---
Surface Footage: The Starting Point
You don't actually start with RPM. You start with Surface Feet per Minute (SFM) — also called cutting speed or surface speed.
SFM describes how fast the cutting edge is moving through the material. This is what determines whether the tool cuts cleanly or generates too much heat. Different materials have recommended SFM ranges based on decades of empirical testing.
Common SFM starting points (solid carbide tools):
| Material | SFM Range |
|---|---|
| Aluminum (6061) | 600 – 1,500 SFM |
| Brass / Bronze | 300 – 700 SFM |
| Mild Steel (1018) | 200 – 400 SFM |
| Stainless Steel (304) | 100 – 250 SFM |
| Titanium | 100 – 200 SFM |
| Hard Steel (D2, H13) | 50 – 150 SFM |
| Plastics (Delrin, nylon) | 500 – 1,000 SFM |
These are starting ranges. Your specific tool manufacturer will give you more precise numbers for their geometry and coating. These are the ballparks.
---
From SFM to RPM
Once you know the target SFM, you calculate the required RPM from your tool diameter:
```
RPM = (SFM × 3.82) / Tool Diameter (inches)
```
The 3.82 comes from 12/π — it converts from the relationship between surface speed, diameter, and rotational speed.
Example: 1/2" (0.500") endmill cutting 6061 aluminum. Target SFM = 1,000.
```
RPM = (1,000 × 3.82) / 0.500
RPM = 3,820 / 0.500
RPM = 7,640 RPM
```
Round to 7,500 or 8,000 depending on your machine's capabilities and your comfort level.
Metric version (using surface speed in m/min):
```
RPM = (Surface Speed m/min × 1,000) / (π × Tool Diameter mm)
```
---
Chip Load: The Other Critical Variable
Chip load is the thickness of material each cutting edge removes per revolution — measured in inches per tooth (IPT).
Chip load matters because:
- • Too little: The tool rubs instead of cuts, generating heat without removing material. Tool wears fast, finish suffers.
- • Too much: Excessive cutting forces — tool deflects, breaks, or chatters.
- • Just right: Clean, efficient cuts that curl off as proper chips, carrying heat with them.
Recommended chip load depends on tool diameter, material, and number of flutes. Your tool manufacturer's speeds and feeds chart will list chip load recommendations. General starting points for carbide in aluminum:
| Tool Diameter | Chip Load (IPT) |
|---|---|
| 1/8" (3mm) | 0.0005 – 0.001" |
| 1/4" (6mm) | 0.001 – 0.002" |
| 1/2" (12mm) | 0.002 – 0.004" |
| 3/4" (19mm) | 0.003 – 0.006" |
Steel chip loads are generally lower — roughly half these values to start.
---
From Chip Load to Feed Rate
Once you have RPM and chip load, feed rate is straightforward:
```
Feed Rate (IPM) = RPM × Chip Load (IPT) × Number of Flutes
```
Continuing the example: 1/2" endmill, 4-flute, 7,640 RPM, chip load 0.003" IPT
```
Feed Rate = 7,640 × 0.003 × 4
Feed Rate = 91.7 IPM
```
Call it 90 IPM to start. That's your programmed F word in the G-code: `F90.0`
---
Depth of Cut: Axial and Radial
Two more parameters define how aggressively you're cutting:
Axial Depth of Cut (ADOC) — how deep the tool goes in Z. For roughing aluminum with a solid carbide endmill, a common starting point is 1× tool diameter as ADOC (1/2" deep with a 1/2" endmill).
Radial Depth of Cut (RDOC) — how much of the tool's diameter is engaged in the cut. For a conventional slotting pass, RDOC = tool diameter (100% engagement). For an adaptive/trochoidal toolpath, RDOC might be only 10–20% of diameter, allowing much higher feed rates.
The combination of ADOC and RDOC determines Material Removal Rate (MRR):
```
MRR (cubic inches/min) = ADOC × RDOC × Feed Rate
```
Higher MRR = faster cycle time = more chips per minute. The limit is machine rigidity, tool deflection, and available spindle power.
---
High-Efficiency Milling (HEM / Adaptive Clearing)
Traditional milling used full-width slotting passes at conservative feeds. Modern CNC practice — especially with adaptive clearing toolpaths in Fusion 360 or Mastercam — uses a completely different approach:
- • Narrow radial engagement (10–20% of tool diameter)
- • Full axial depth (1–2× tool diameter)
- • Higher feed rates (possible because of lower cutting forces at low RDOC)
- • Consistent tool engagement (the toolpath constantly adjusts to maintain contact angle)
The result: dramatically higher material removal rates, much lower cutting forces, far less heat, and greatly extended tool life. Fusion 360 calls this "Adaptive Clearing." Mastercam calls it "Dynamic Mill." The concept is the same.
Learning adaptive clearing toolpaths is one of the highest-leverage skills in modern CNC machining. Once you understand the feeds/speeds math, this is what to learn next.
---
What Happens When Things Go Wrong
Chatter: A squealing, rattling vibration. The tool is deflecting and bouncing. Causes: too high feed rate, too large RDOC, tool sticking out too far from holder, workpiece not clamped rigidly. Fix: reduce feed rate and/or RDOC, increase spindle speed slightly, use shorter tool.
Built-up edge (BUE): Material from the workpiece welds onto the cutting edge. Common in aluminum and stainless at too-low cutting speeds. Tool starts to smear rather than cut. Fix: increase SFM. Make sure you have proper lubrication.
Burned tool: Tip turns blue/black, finish degrades, tool is dull. Cause: excessive heat — usually from too-low feed rate (dwelling and rubbing) or running without coolant in materials that need it. Fix: increase feed rate, add coolant.
Snapped tool: Sudden fracture. Cause: too high chip load, unexpected hard spot in material, excessive ADOC, tool collision. Fix: reduce chip load, verify program, check workholding.
Blue chips in steel: Discolored chips mean the material is hot. Adjust feeds/speeds and coolant to bring heat under control.
Long stringy chips in aluminum: "Bird nesting" around the tool. Usually means feed rate is too low for the chip to break properly. Increase feed rate or use a 2-flute endmill with better chip evacuation.
---
The "Feel" You Develop
Here's the honest truth about feeds and speeds: the math gives you a starting point. Experience gives you the instinct to optimize from there.
After years in my shop, I could walk up to a running machine and hear whether the cut sounded right. A good cut has a certain pitch and rhythm — a steady hum with consistent chip formation sounds and smell. A cut about to break a tool has a different character — a higher pitched screech, irregular harmonics, or an unusual silence.
You develop this. It takes time and it takes running the machines. Start with the calculated numbers, watch and listen carefully, and adjust incrementally. Document what worked. Over time the math becomes intuition.
Use tools like Kennametal's NOVO, Harvey Tool's speeds and feeds calculator, or Fusion 360's built-in calculator to generate starting numbers. Then learn to read the cut.
---
Quick Reference Summary
| Parameter | Formula |
|---|---|
| RPM from SFM | `(SFM × 3.82) / Diameter` |
| Feed Rate | `RPM × Chip Load × Flutes` |
| MRR | `ADOC × RDOC × Feed Rate` |
Keep these formulas handy. After a while, you'll know the typical numbers for your common materials and tool sizes by memory.
Next and final post in the series: coolant, workholding, and the physical setup of a job from blank material to first cut.
— Dr. Scott