Chip Thinning, HEM & HSM Strategies
Chip thinning is the most misunderstood concept in modern milling. When your radial engagement drops below 50% of the cutter diameter, the actual chip becomes thinner than what you programmed. If you do not compensate by increasing your feed rate, you are rubbing instead of cutting — wasting time, burning tools, and making terrible noises. This article explains the physics, gives you the formulas, and covers the two dominant strategies that exploit chip thinning: High Efficiency Machining (HEM) and High Speed Machining (HSM).
The Chip Thinning Problem
What Happens at Low Radial Engagement
When an end mill takes a full-width slot (radial engagement = 100% of diameter), the chip thickness equals the programmed feed per tooth. The thickest point of the chip is at the center of the cutter path.
But when you reduce radial engagement — say to 25% of the cutter diameter — the geometry changes. The insert or flute does not sweep through as much arc, so the chip never reaches the full programmed thickness. The maximum chip thickness is significantly less than the feed per tooth you programmed.
This means:
- You are cutting a thinner chip than intended
- The thinner chip carries less heat away from the cutting edge
- The tool rubs more than it cuts
- Tool life decreases (counterintuitively — you would think lighter cuts would be easier on the tool)
- Surface finish degrades from the rubbing
- You are wasting cycle time because MRR is lower than it should be
The Fix: Increase Feed
Increase feed when radial engagement drops below 50%. This is not optional — it is required to maintain proper chip thickness and cutting action.
The purpose of chip thinning compensation is to maintain the same effective chip thickness regardless of radial engagement. You increase the programmed feed per tooth so the actual chip thickness equals your target chip load.
The Chip Thinning Formula
The exact relationship between programmed feed, radial engagement, and actual chip thickness:
Effective Chip Thickness
hex = fz x sqrt(ae / D) (simplified, for ae < 50% of D)
Where:
- hex = effective (actual) chip thickness
- fz = programmed feed per tooth
- ae = radial depth of cut (stepover)
- D = cutter diameter
Adjusted Feed Per Tooth (Compensated)
To achieve your target chip thickness, use:
fz_adjusted = fz_target / sqrt(ae / D)
Or equivalently:
fz_adjusted = fz_target x sqrt(D / ae)
Example: You want a 0.003" chip load with a 0.500" end mill at 10% engagement (ae = 0.050"):
fz_adjusted = 0.003 x sqrt(0.500 / 0.050) = 0.003 x sqrt(10) = 0.003 x 3.16 = 0.0095" per tooth
So you would program approximately 0.0095" per tooth to actually cut a 0.003" chip.
Practical Adjustment Factors
You do not need to calculate the square root every time. Use this table for common radial engagements:
| Radial Engagement (% of D) | ae/D Ratio | Feed Multiplier | Effective Result |
|---|---|---|---|
| 50% | 0.50 | 1.0x (no adjustment) | Chip = programmed feed |
| 40% | 0.40 | 1.12x | Slight increase needed |
| 30% | 0.30 | 1.3x | Moderate increase |
| 25% | 0.25 | 1.4x | |
| 20% | 0.20 | 1.6x | |
| 15% | 0.15 | 1.8x | |
| 10% | 0.10 | 2.2-3.0x | Significant increase — increase feed |
| 5% | 0.05 | 3.5-5.0x | Major increase — feed must be 4-5x baseline |
| 3% | 0.03 | 5-6x | Extreme — common in HSM finishing |
Key takeaway: At 10% radial engagement, you need to roughly triple your feed rate. At 5% engagement, increase feed by 4-5x. If you do not, you are rubbing.
HEM — High Efficiency Machining
HEM (also called High Efficiency Milling or Dynamic Milling) is a roughing strategy that uses full axial depth, low radial engagement, and high feed rate to maximize metal removal while keeping cutting forces and heat under control.
HEM Parameters
| Parameter | HEM Approach | Conventional Approach |
|---|---|---|
| Axial depth (ADOC) | Full flute length (1xD to 2xD) | 0.5xD to 1xD |
| Radial depth (RDOC) | 5-15% of D | 50-100% of D |
| Feed per tooth | 2-5x conventional (chip thinning compensated) | Manufacturer recommended |
| SFM | Same or slightly higher than conventional | Manufacturer recommended |
| Toolpath | Trochoidal, adaptive, or constant-engagement | Linear, zigzag |
Why HEM Works
- Low radial engagement means each flute takes a thin chip, generating less heat per tooth
- Full axial depth uses the entire cutting edge, distributing wear evenly (no "one spot" wear)
- High feed (compensated for chip thinning) maintains proper chip thickness and MRR
- Constant engagement (via trochoidal or adaptive paths) prevents the sudden load spikes that break tools
- More flutes engaged at full depth = higher IPM at the same chip load per tooth
HEM Example
Material: 4140 steel, roughing a pocket Tool: 0.500" 5-flute carbide end mill
| Parameter | Conventional | HEM |
|---|---|---|
| ADOC | 0.250" | 1.000" (2xD) |
| RDOC | 0.250" (50%) | 0.050" (10%) |
| FPT | 0.003" | 0.009" (3x, chip thinning compensated) |
| SFM | 400 | 450 |
| RPM | 3,056 | 3,438 |
| IPM | 45.8 | 154.7 |
| MRR | 2.86 in^3/min | 7.73 in^3/min |
HEM removes 2.7x more material per minute despite cutting a narrower slot, because the feed rate is tripled and the axial depth is quadrupled.
When to Use HEM
- Roughing operations with significant material to remove
- Pockets, profiles, and open roughing
- When machine has adequate spindle power and feed rate capability
- CNC machines with modern controls that can handle constant-arc toolpaths (lookahead)
When NOT to Use HEM
- Thin-wall parts that cannot take full-depth loads
- Machines with slow axis acceleration (the constant direction changes will slow actual feed below programmed)
- Very small features where the toolpath overhead exceeds the benefit
- When the programmer is not comfortable with adaptive toolpaths
HSM — High Speed Machining
HSM is a finishing strategy that uses light axial depth, light radial engagement, and very high speed/feed to produce near-net-shape surfaces with excellent finish.
HSM Parameters
| Parameter | HSM Approach |
|---|---|
| Axial depth (ADOC) | 0.010" to 0.050" (light) |
| Radial depth (RDOC) | 5-15% of D |
| SFM | 50-100% higher than conventional |
| Feed per tooth | 2-5x conventional (chip thinning compensated) |
| Toolpath | Constant stepover, smooth curves, no sharp corners |
HSM vs. HEM — The Key Difference
| HEM (Roughing) | HSM (Finishing) | |
|---|---|---|
| Goal | Maximum MRR | Best surface finish + accuracy |
| ADOC | Full flute length | Very light |
| RDOC | Low (5-15%) | Low (5-15%) |
| Speed | Normal or slightly high | Very high |
| Feed | High (chip thinning compensated) | High (chip thinning compensated) |
| Result | Fast roughing | Smooth finishing |
Both strategies use chip thinning compensation. Both use low radial engagement. The difference is HEM goes full-depth for MRR, while HSM goes light-depth for finish quality.
Trochoidal Milling — The HEM Toolpath
Trochoidal milling is the toolpath that makes HEM possible. Instead of cutting a straight slot, the tool follows a circular/spiral path that maintains constant radial engagement.
How Trochoidal Milling Works
- The tool plunges or ramps into the material
- It follows an arc or spiral path that sweeps through a narrow width (5-15% of D)
- At the end of each loop, the tool advances forward by the stepover amount
- The cycle repeats, creating a slot wider than the tool diameter
Trochoidal Milling Parameters
| Parameter | Starting Point | Notes |
|---|---|---|
| Stepover | 5-15% of tool diameter | Lower for harder materials |
| ADOC | 1x to 2x tool diameter | Use full flute length |
| SFM | Same as conventional | Can increase 10-20% |
| FPT | 2-5x conventional (compensated) | Must increase feed |
| Arc radius | Tool radius + stepover | Controls engagement angle |
Programming Trochoidal Paths
Most modern CAM systems support trochoidal/adaptive toolpaths:
- Fusion 360: Adaptive Clearing
- Mastercam: Dynamic Milling / OptiRough
- SolidCAM: iMachining
- HSMWorks: Adaptive Clearing
- GibbsCAM: VoluMill
These CAM systems automatically calculate the chip thinning compensation and adjust feed rates based on engagement angle. If your CAM does not support this, you must manually calculate the adjusted feed.
Full-Width Slotting vs. Low-Engagement Roughing
Full-Width Slotting (100% Radial Engagement)
- Chip thickness equals programmed FPT — no chip thinning
- Maximum cutting force on the tool
- Maximum heat generation (chip takes limited heat away)
- Fastest for narrow slots where you must cut a full-width slot
- Reduce ADOC to 0.5-1.0x tool diameter to manage forces
- Use 2-3 flute tools for chip evacuation
Low-Engagement Roughing (10-15% Radial)
- Chip is thinner than programmed — must increase feed to compensate
- Lower cutting force per tooth
- Better heat management (each tooth cools between engagements)
- Use full ADOC (1-2x tool diameter)
- Use 4-7 flute tools (more flutes = higher IPM at same FPT)
- Higher overall MRR despite narrower cut width
Which is Faster?
For removing a large volume of material, low-engagement roughing with chip thinning compensation is almost always faster than full-width slotting. The math:
Full-width slot: 0.500" tool, 0.250" ADOC, 50% engagement, 3 flutes, 0.003 FPT, 3000 RPM
- IPM = 3000 x 0.003 x 3 = 27 IPM
- MRR = 0.500 x 0.250 x 27 = 3.38 in^3/min
Trochoidal (same tool): 0.500" tool, 1.000" ADOC, 10% engagement (0.050"), 3 flutes, 0.009 FPT (3x compensated), 3000 RPM
- IPM = 3000 x 0.009 x 3 = 81 IPM
- MRR = 0.050 x 1.000 x 81 = 4.05 in^3/min
The trochoidal approach wins by 20% in MRR, with less tool stress. With a 5-flute tool (which you can use at low engagement because chip evacuation is easier), the advantage grows further.
Common Mistakes
1. Not Increasing Feed at Low Engagement
This is the number one mistake. A programmer sets up a 10% stepover adaptive path and leaves the feed at the manufacturer's recommended 0.003" FPT. The actual chip is only 0.001" — the tool is rubbing, not cutting. Increase feed to compensate.
2. Using Full Engagement Feed at Low Engagement
Same problem. If your chip load table says 0.003" per tooth, that is for 50%+ radial engagement. At 10%, you need 0.007-0.009" per tooth.
3. Exceeding Machine Feed Rate Capability
HEM and trochoidal paths require high feed rates — sometimes 200+ IPM. If your machine cannot accelerate fast enough to maintain these rates through tight arcs, the actual feed drops and the tool rubs. Check your machine's actual feed rate (not programmed) during trochoidal operations.
4. Using HEM Feeds with Full-Width Engagement
If you compensate feed for 10% engagement and then the toolpath makes a full-width cut (inside corner, for example), the chip load quadruples and the tool snaps. Good CAM systems handle this by reducing feed at high-engagement areas. If yours does not, add a maximum engagement limit.
5. Ignoring ADOC Limits
HEM uses full flute length for ADOC. But some end mills have shorter length of cut (LOC) than the flute length. Do not exceed the LOC, and do not bury the shank in the cut.
Quick Start Guide — Setting Up HEM
-
Choose the right tool: 4-7 flute carbide end mill with variable helix (reduces chatter at full depth). Long LOC (at least 2xD).
-
Set ADOC: 1x to 2x tool diameter (use full LOC if geometry allows)
-
Set RDOC: Start at 10% of tool diameter
-
Look up baseline FPT for the material (see [[speeds-feeds-reference]])
-
Apply chip thinning multiplier: At 10% engagement, multiply FPT by approximately 3x
-
Calculate IPM: RPM x adjusted FPT x number of flutes
-
Set SFM: Use the normal range for the material (or 10-15% higher)
-
Program the toolpath: Use adaptive/trochoidal clearing in your CAM system
-
Run it: Listen for smooth cutting (consistent pitch, no squealing). If it sounds scratchy or intermittent, feed is too low — increase feed.
-
Check the chips: They should be small, consistent crescent shapes. Long stringy chips mean feed is too low. Powder or dust means feed is WAY too low.
Key Takeaways
- When radial engagement drops below 50%, increase feed to maintain proper chip thickness — this is non-negotiable
- At 10% engagement, feed should be approximately 3x the full-engagement value
- At 5% engagement, feed should be approximately 4-5x the full-engagement value
- HEM = full depth + low radial + high feed = best roughing strategy for most materials
- HSM = light depth + low radial + very high speed + high feed = best finishing strategy
- Trochoidal milling is the toolpath that enables HEM by maintaining constant engagement
- Modern CAM systems handle chip thinning compensation automatically — but verify the numbers
- Full-width slotting at reduced depth is rarely faster than trochoidal at full depth
Related Articles
- [[speeds-feeds-reference]] — SFM and FPT values by material (the starting point before chip thinning adjustment)
- [[trochoidal-adaptive-milling]] — Detailed trochoidal toolpath programming
- [[slotting]] — Full-slot cutting strategies
- [[endmill-types]] — End mill selection for HEM and HSM applications