The most common frustration for a CNC milling operator is: “I set the right feed, yet the tool wore out fast, the surface degraded or the part chattered.” The reason is usually chip thinning: the fz you type on the machine and the maximum chip thickness the cutting edge actually sees (hex) are not the same. The Mentor CNC tool below calculates that gap for you and explains what it means for tool life, cycle time and part quality.
MENTOR CNC CALCULATOR • CNC MILLING
CNC Milling Maximum Chip Thickness (hex) and Chip Thinning Calculator
The feed you type on the machine and the chip thickness the cutting edge actually sees are not the same. That gap is the invisible cause of inserts that wear out early, poor surfaces, chatter and needlessly long cycle times. The Mentor CNC hex tool calculates the real maximum chip thickness from diameter, radial width, axial depth and approach angle — so you extend tool life, raise feed safely, and get the part right the first time.
What does this hex calculator give a CNC operator?
You enter feed and speed on the machine; but the chip thickness the cutting edge actually sees is often not the value you typed. This gap is the hidden reason behind those moments when you say “I did everything right, yet the tool wore out early / the surface came out poor / the part chattered.” This tool calculates the real maximum chip thickness (hex) from your inputs and gives you these concrete gains:
Extends tool life
At a very low chip thickness the cutting edge rubs instead of cutting; heat and wear accelerate. The tool shows whether you are in the rubbing zone so you don't burn the insert out early.
Shortens cycle time
At low radial engagement or with a 45° / high-feed cutter the chip thins. By accounting for this thinning you raise the feed safely and finish the same part faster.
Reduces scrap and rework
Too much hex brings edge chipping and vibration; too little brings dimensional and surface problems. Staying in the right window gets the part right the first time.
Helps you pick the right cutter
Compare 90°, 45°, high-feed and round-insert cutters on the same hex and choose the best tool and feed for the job in advance.
Adapts the catalog value to your part
Enter the manufacturer's “target hex” and the tool back-calculates the fz feed needed for your diameter, depth and angle.
Explains why
Every result comes with an operator-specific note: why it thinned, what the risk is, what to check. You get decision support, not just a number.
How to use it in 3 steps
Describe the cutter
Pick the operation (side, face, slot, round nose…) and the cutting geometry. The tool opens only the fields you need for that choice.
Enter 3 core values
Feed per tooth fz, cutter diameter Dc, radial width ae and axial depth ap. That's all hex needs.
Read and apply
Get hex, the chip-thinning percentage and the operator note. If needed, set your feed safely using the target hex.
Mentor CNC Milling Maximum Chip Thickness hex Calculator
First select the cutter geometry. The tool opens only the fields required for the selected geometry.
Operation assessment
3 real shop examples: what does hex tell you?
The three typical cases below show why the same feed gives different results under different conditions, and how the tool guides you.
1) Ø20 end mill with a thin side pass — “why did the tool wear out so fast?”
A Ø20 cutter takes only a 1 mm side pass (ae=1 mm): ae/Dc = 5%. You entered fz=0.10 mm/tooth on a 90° cutter. The tool calculates hex as about 0.044 mm — the cutting edge sees less than half of what you entered. This is the rubbing and work-hardening zone. Gain: raise the feed in a controlled way so the insert really cuts, improving tool life and surface.
2) 45° face mill — “why does the same F cut lighter?”
You use fz=0.20 mm/tooth on your face mill. The 45° approach angle thins the chip; hex becomes about 0.141 mm. So there is still headroom on the cutting edge. Gain: you can run a higher fz than a 90° tool to boost productivity, while lower radial force deflects a thin wall less.
3) Ball nose with a shallow pass — “the math looks fine but the surface is poor”
You work with ap=0.5 mm on a Ø12 ball nose: ap/iC = 4%. Because the effective approach angle drops sharply, the chip thins significantly. Gain: the tool warns you that you are in this “thinning zone”; raise the feed accordingly or adjust the depth of cut, avoiding both rubbing and vibration-driven surface waviness.
How do metal removal and chip formation happen in milling?
In turning, the workpiece usually rotates and the cutting tool cuts continuously. In milling, the cutting tool rotates; each cutting edge on the tool enters the workpiece, removes a chip and leaves the cut again. For this reason milling is an interrupted cutting operation. As each cutting edge enters the cut it takes an impact load, carries a chip thickness that changes throughout the cut, and is released from the load at exit.
For one edge on the cutter, the chip thickness is not constant in most operations. Depending on the rotation angle of the tool, how far it enters the part and the feed direction, it can rise from near zero to a maximum, or drop from the maximum to zero. For this reason the feed per tooth fz entered on the machine and the maximum chip thickness hex that the cutting edge actually sees are not always the same.
Entry into the cut
The cutting edge contacts the workpiece. The entry shape affects impact, edge load and tool life.
Chip formation
The uncut metal layer is compressed, deforms and flows along the cutting face to become a chip.
Chip evacuation
The formed chip must leave the cutting zone. Otherwise the next edge can recut the chip.
Is measuring the milling chip with a caliper an hex measurement?
No. During cutting the chip is compressed, heats up, deforms plastically and curls. For this reason the thickness of the chip leaving the machine, measured with a caliper, is not equal to the theoretical metal layer before it was cut. hex is not the physical size of the removed chip; it is the theoretical maximum uncut chip thickness that the cutting edge encounters during a cut.
What do ap, ae, Dc, fz, zc and Vf mean in milling calculations?
Knowing what each field in the calculator represents is the first condition for getting the correct result. The abbreviations below may look similar but describe different measurements.
Cutter cutting diameter — Dc, mm
Dc is the diameter of the cutting cutter. If you use a Ø50 face mill, Dc=50 mm. On ball-nose tools, the nominal diameter and the actual cutting diameter may not be the same at every contact point; the closer you get to the tool center, the lower the actual cutting speed.
Axial depth of cut — ap, mm
ap shows how far the cutter plunges into the part along the tool axis, in the Z direction on most vertical machining centers. If you machine 2 mm below the top surface of the part, ap=2 mm. In side milling, ap can also be thought of as the working height of the peripheral cutting edge of the cutter in the part.
Radial width of cut — ae, mm
ae shows how far the diameter of the cutter enters the part sideways; it is not the diameter of the cutter. For example, if the cutter is Ø50 mm but removes a pass only 25 mm wide from the part, ae=25 mm. In this case ae/Dc=25/50=50%. If a Ø20 end mill removes only a 1 mm side pass, ae/Dc=5% and significant radial chip thinning can occur.
Feed per tooth — fz, mm/tooth
fz is the theoretical feed load taken by each cutting edge on the tool in one revolution. For example, if fz=0.10 mm/tooth, spindle speed is 2,000 rpm and the effective number of teeth is 4, the table feed is approximately 0.10×2,000×4=800 mm/min. fz is not the mm/min value entered directly on the machine.
Effective number of teeth — zc
zc is the effective number of teeth used in the calculation. Having 6 inserts on the tool body does not always mean 6 inserts are in the cut at the same time. In the table feed calculation, the effective number of teeth recommended by the manufacturer or the total number of working teeth of the tool must be used.
Table feed — Vf, mm/min
Vf shows how many millimeters per minute the machine advances on the X, Y or Z axes. The basic relationship is Vf=fz×zc×n. The hex calculation is made over the feed per tooth; if only the mm/min value is known, fz=Vf/(zc×n) must be found first.
ae: lateral width of cut in top view
If the cutter diameter is 50 mm and the working lateral width in the part is 25 mm, the engagement is 50%.
ap: depth in the Z direction in side view
If 2 mm of stock is removed in the Z direction from the top surface, ap=2 mm.
What is chip thinning in milling and why is it important?
Chip thinning is the reflection of the programmed fz value onto the cutting edge as a smaller hex, due to tool geometry or low cutting engagement. If very low feed is used without knowing about chip thinning, the cutting edge may not reach a sufficient chip thickness; it can rub instead of cutting, and heat and wear can increase. If the geometric correction is applied correctly, the table feed can be increased while keeping the same cutting edge load.
1. Chip thinning due to the approach angle
On straight-edged cutters, the basic geometric relationship is hex=fz×sin(KAPR). When KAPR is 90°, hex is approximately equal to fz. As the angle decreases, the chip forms thinner and wider. For example, for fz=0.20 mm/tooth, a 45° cutter produces only about 0.141 mm maximum chip thickness. On a 10° high-feed geometry, the theoretical fz for the same hex can be much higher; but the tool manufacturer's maximum ap and fz limits must not be exceeded.
| KAPR | Geometry factor | hex for fz=0.20 | General usage comment |
|---|---|---|---|
| 90° | 1.000 | 0.200 mm | Side and slot milling; hex≈fz |
| 75° | 0.966 | 0.193 mm | Slight thinning |
| 65° | 0.906 | 0.181 mm | Load distribution in face milling |
| 45° | 0.707 | 0.141 mm | Significant thinning and low radial force |
| 10° | 0.174 | 0.035 mm | High-feed geometry with small ap |
2. Chip thinning due to low radial width of cut
In peripheral or side milling, when the ae/Dc ratio drops below 50%, the cutting edge can leave the cut before reaching the maximum fz thickness. The approximate radial thinning factor can be expressed as 2×√[(ae/Dc)×(1−ae/Dc)]. If the engagement is 50% or higher, the factor is taken as at most 1.
For example, when a 1 mm side pass is taken with a Ø20 end mill, ae/Dc=5%. The radial factor is approximately 0.436. If fz=0.10 mm/tooth is entered on a 90° tool, the theoretical hex can be about 0.044 mm. To keep the same target hex, fz can be increased geometrically; however, the tool, machine, surface quality and manufacturer limits must also be verified.
3. Chip thinning due to low ap on a round or ball nose
On round-insert cutters and ball-nose end mills there is no fixed approach angle. The point where the cutting edge contacts the part changes depending on the ap value. As the ap/iC ratio decreases, the effective approach angle decreases and the chip thins. On round inserts, keeping ap below about 25% of the insert diameter is a clear thinning zone that keeps the effective approach angle below 60°.
For round or ball geometry, the basic factor can be calculated as √[(4ap/iC)−(2ap/iC)²]. On a ball nose, the nominal tool diameter is used instead of iC; but since the actual cutting speed is very low near the tool center, the hex calculation alone is not sufficient.
How do climb and conventional milling change chip formation?
Climb milling — down milling
The rotation direction at the cutter contact point is the same as the table feed direction. In peripheral climb milling, the chip starts thick at the beginning of the cut and approaches zero at exit. The cutting edge cuts directly at the start; the tendency to rub on the surface for a long time is reduced. On modern backlash-free CNC machines, this is the basic preference in most applications.
- Larger chip thickness at the start
- Less friction and less sliding on the work-hardened surface
- Cutting forces can help press the part into the fixture
- Requires caution on older systems with table backlash
Conventional milling — up milling
The rotation direction at the cutter contact point is opposite to the table feed. The chip starts at near zero thickness and thickens toward exit. The cutting edge can rub on the surface at the first moment; temperature, wear and work hardening can increase. The thick chip at exit can strain the cutting edge.
- Thin chip at entry and risk of friction
- High chip thickness and edge load at exit
- Cutting forces can tend to lift the part off the table
- Can be preferred with variable stock or some ceramic applications
How do the cutter type and approach angle affect the hex calculation?
90° shoulder mills and end mills
90° cutters are versatile; they are used in shoulder creation, slot, pocket and peripheral milling. On a straight-edged 90° geometry there is no angle-based chip thinning. However, if the ae/Dc ratio is below 50%, radial thinning can still occur.
45° face mills
45° face mills make the chip thinner and wider. A larger portion of the cutting force is created in the axial direction; this can increase productivity in rigid face milling applications and reduce radial deflection on some thin-walled parts. For the same hex, a higher fz may be needed than with a 90° tool.
10°–20° high-feed mills
A very small approach angle converts only a small part of the programmed feed into chip thickness. That is why high-feed mills can work with high fz values per tooth. In return, ap must usually be kept small. The small angle carries the cutting force largely into the axial direction; the spindle, clamping and tool body capacity must be checked.
Round-insert and large-radius cutters
Round inserts provide a strong cutting edge and a long contact length. Since the effective approach angle changes with ap, the round insert diameter iC is required in the hex calculation. At low ap values, significant chip thinning occurs; as ap increases, the effective angle and chip thickness rise.
Ball-nose end mills
Ball noses are used in 3D mold and profile milling. At the tool center, the peripheral speed theoretically approaches zero. Tilting the tool or moving the contact point away from the center can increase the actual cutting diameter. This tool estimates hex for simple contact geometry; in 3- and 5-axis tool tilt, the CAM system's actual contact and feed calculation must also be checked.
Why are material, chip evacuation, tool runout and rigidity as important as hex?
ISO P — Steel
Medium and long chips can form. Controlled chip evacuation is targeted with suitable geometry, fz, ap and ae.
ISO M — Stainless steel
There is a risk of sticky chips, work hardening and high heat. A very low hex can increase friction and edge build-up.
ISO K — Cast iron
It usually produces short, brittle chips. The effect of dust and abrasive particles on the machine guard must be considered.
ISO N — Aluminum and non-ferrous materials
A wide chip space, a sharp and polished cutting edge and good evacuation are important. If the chip fills the pocket, it can be recut.
ISO S — Titanium and nickel alloys
Temperature and load at the cutting edge are intense. Small radial engagement, a controlled toolpath and the correct coolant strategy become important.
ISO H — Hardened materials
Cutting edge stress is high. Impact-free entry, low runout, short tool overhang and stable hex can be critical.
Recutting of the chip
In pocket, slot and deep cavity operations, if the chip cannot be ejected, the next cutting edge hits the previously formed chip. This creates an additional and irregular impact load outside the calculated hex. Compressed air, internal coolant, a suitable helix and sufficient chip space must be evaluated according to the operation type.
Tool runout and load sharing between teeth
If one cutting edge is positioned higher than the others due to runout, the teeth do not share the fz load that should theoretically be equal. The high tooth can remove a thicker chip than the calculated hex, while the other teeth rub. The collet, holder, tool seat, insert pocket and spindle runout must be checked.
Tool overhang and vibration
Long tool overhang rapidly reduces rigidity. When the cutter deflects under cutting force, the actual ae and hex can change continuously. As a result, vibration, surface waviness, corner breakage and dimensional error can occur. Even if the calculation is correct, a safe result should not be expected if the mechanical system is unstable.
What should you do if you do not know the milling speed and feed?
The hex calculation requires the feed per tooth fz. The fz value can be found on the insert box or in the manufacturer catalog. If you only have the Vf mm/min value written on the machine, you can find the feed per tooth with the formula fz=Vf/(n×zc).
To calculate feed and speed together, you can use the Mentor CNC CNC speed and feed calculator. That tool calculates Vc, spindle speed and feed together for turning, milling and drilling operations.
Milling Speed and Feed CalculatorIf there is a chip, vibration or insert problem in milling, in what order should you check?
- fz: Is the feed per tooth too low, is the cutting edge rubbing instead of cutting?
- ae/Dc: Was chip thinning accounted for at low radial engagement?
- KAPR: Was fz corrected properly on a 45° or high-feed geometry?
- ap: On a round/ball nose, are the effective angle and the tool's maximum depth of cut suitable?
- Chip evacuation: Are chips staying in the pocket and being recut?
- Runout: Is one cutting edge carrying more load than the others?
- Tool overhang: Is the tool longer than necessary, are the holder and spindle connection rigid?
- Milling direction: Is the climb/conventional selection suitable for the machine and fixture?
- Vc and temperature: Is the cutting speed suitable for the material and insert grade?
- Cutting geometry: Is there enough chip space for a full slot, long-chipping material or heavy cut?
Common calculation mistakes
- Thinking the ae value is the cutter diameter; assuming a Ø50 cutter always works at ae=50.
- Confusing ap with ae; entering the lateral pass value instead of the Z depth.
- Entering the F800 mm/min written on the machine directly as fz=800.
- Overlooking radial chip thinning in a low ae operation.
- Using a large ap on a 10° high-feed mill.
- Assuming that when cutting from the tool center with a ball nose, the nominal Vc occurs at the actual contact point.
- Neglecting tool runout and single-tooth overload even if the calculated average load is suitable.
- Evaluating the calculated hex independently of mechanical rigidity with a long tool overhang.
Frequently asked questions
Are hex and fz the same in milling?
They can be equal or very close only in some 90° geometries and with sufficient cutting engagement. With a small KAPR, low ae/Dc or a round nose, hex can be smaller than fz.
Why can ae be smaller than the cutter diameter?
The cutter may machine only one edge of the part, not the whole part. If a Ø50 cutter removes a 10 mm side pass from the part, ae=10 mm and the engagement is 20%.
If there is chip thinning, is the feed always increased?
No. It can be increased geometrically; but the insert, tool body, ap, surface quality, machine acceleration, power, rigidity and manufacturer limits must also be checked.
Why can a very low hex be harmful?
If the cutting edge cannot enter a sufficient metal layer, it can rub instead of cutting. This can create heat, surface deterioration, work hardening and rapid wear.
What does a very high hex lead to?
If the capacity of the cutting edge is exceeded, micro-chipping, corner breakage, body load, vibration or a machine power limit problem can occur.
This tool is prepared for geometric calculation and training purposes. The calculated hex is not the exact working range recommended by the tool manufacturer. Insert grade, geometry, coating, tool body, maximum ap, machine power, spindle speed, clamping, runout, tool overhang and chip evacuation can change the result. The first trial should be performed on a guarded machine, with safe starting values and stepwise control.