Let's start with a counterintuitive conclusion: when a desktop CNC cuts carbon fiber, the feed rate limit is almost never the bottleneck; the spindle speed limit is. Converting Harvey Tool's published composite cutting data, a reasonable feed for high-fiber-content CFRP is on the order of 500–800 mm/min, far below the machine's 2,500 mm/min limit. What actually hits the ceiling is the spindle speed required when small tool diameters meet high cutting speeds.
The One-Minute Summary
- You won't use up a 2,500 mm/min feed limit. Per Harvey Tool data, CFRP with 21–40% fiber content needs only 510–800 mm/min with 2–6 mm tools.
- The 20,000 rpm spindle limit becomes a constraint in two cases: low-fiber-content material (5–20%, SFM 500–700) needs over 24,000 rpm with a 2 mm tool, and 22,600 rpm with a 3 mm tool.
- The reason for "high speed, low feed, shallow depth of cut" is that CFRP does not form continuous chips; the fibers and resin fail by brittle fracture. Lowering feed per tooth reduces cutting force, temperature, and tool deflection all at once.
- There is experimental data on thermal thresholds: subsurface thermal damage begins at a workpiece temperature of 120°C, and results are best around 80°C (Pecat et al., 2012).
- The climb vs. conventional debate matters little. The dominant variable is the fiber cutting angle θ: with θ between 0 and 90°, even a dull tool does not delaminate; problems appear only at 90–180°.
- A trade-off you must know: parameters that favor surface quality (high speed, low feed) and parameters that favor dust safety point in opposite directions.
Why "High Speed, Low Feed, Shallow Depth of Cut"
When you cut metal, the cutting edge pushes material into a continuous curled chip. Cutting CFRP is nothing like that. Carbon fiber is brittle, and machining it means "breaking" fibers and resin one after another rather than "shaving" them off. A Harvey Performance technical article puts it plainly: machining carbon fiber is not peeling material away but fracturing the fibers and resin.
That difference leads to three principles:
| Principle | Mechanism | What happens if you ignore it | Basis |
|---|---|---|---|
| High spindle speed | More cuts per unit time, so each flute carries a smaller load | Excessive load per tooth; fibers are pushed aside instead of cut | Meshreki et al. (2012), high-speed milling tests |
| Low feed | Lower feed per tooth → lower cutting force, lower temperature, less tool deflection | Delamination worsens markedly once cutting force exceeds about 200 N | Wang et al. (2011) |
| Shallow depth of cut | Fewer fibers engaged at once, limiting axial thrust | Exit-side fibers are pushed out as a whole layer, causing delamination | Hintze et al. (2011) |
The key mechanism comes from Hintze et al., published in 2011 in Composites Science and Technology: when a fiber has not yet reached its transverse failure strain, the cutting edge pushes it aside instead of cutting it. Those pushed-aside fibers are the burrs and uncut fibers you see on the finished edge.
Fiber cutting angle θ and where edge defects occur
The angle of the cutting edge relative to the fiber direction determines whether fibers are cut or pushed aside
135° Is the Worst Angle and 45° the Best: Consensus From Three Independent Studies
Break θ down further and the literature gives a fairly consistent answer to "which angle does the most damage." The three studies below used completely different measurement methods, yet all point to the same conclusion:
| Study | Measurement method | 45° | 90° | 135° |
|---|---|---|---|---|
| Abena et al. (2023) | Spring-back estimated from surface topography | 328 µm | 2,549 µm | 4,902 µm |
| Wang et al. (2017) | 15 MHz scanning acoustic microscopy | Fa 1.20 | Fa 1.001 | Fa 1.99 |
| Hintze & Hartmann (2013) | Anisotropic elasticity calculation | No damage | 0.1–0.2 mm | Up to 0.45 mm |
| The three studies do not agree on 90° (measurement definitions and cutting conditions differ, so absolute values should not be compared across papers), but "135° is worst, 45° is best" is the conclusion all three share. At 135°, the fiber axis "faces into" the tool, bends sharply, and breaks below the cutting plane; after the tool passes, elastic recovery leaves pits behind. | ||||
You cannot keep an entire profile away from 135°, but you can decide which edges fall at which angles. In practice, place the edges with the strictest cosmetic requirements, or those that will later be bonded, on the 0–90° side of the fiber direction, and leave the less important edges to the critical zone. For a rectangular part, aligning the long edges with the 0° fiber direction puts the longest stretch in the safe zone.
Real Parameters Within 20,000 rpm × 2,500 mm/min
The values below are converted from Harvey Tool's Speeds & Feeds product chart (Series 6989xx / 7852xx, diamond-cut end mills for composites), using the row "Carbon/Glass Fiber, 21–40% fiber content," with a recommended cutting speed of SFM 300–400 (91–122 m/min).
| Tool diameter | Operation | Feed per rev | Recommended rpm | Converted feed (mm/min) | Machine feasibility |
|---|---|---|---|---|---|
| Ø2 mm | Slot | 0.036 mm/rev | 14,553–19,404 | 521–695 | Just within the 20,000 limit |
| Ø2 mm | Profile | 0.041 mm/rev | 14,553–19,404 | 597–796 | Just within the limit |
| Ø3 mm | Slot | 0.053 mm/rev | 9,702–12,936 | 510–680 | Ample margin |
| Ø3 mm | Profile | 0.060 mm/rev | 9,702–12,936 | 584–779 | Ample margin |
| Ø4 mm | Slot | 0.071 mm/rev | 7,277–9,702 | 513–684 | Ample margin |
| Ø4 mm | Profile | 0.081 mm/rev | 7,277–9,702 | 588–784 | Ample margin |
| Ø6 mm | Slot | 0.106 mm/rev | 4,851–6,468 | 513–683 | Ample margin |
| Ø6 mm | Profile | 0.120 mm/rev | 4,851–6,468 | 584–778 | Ample margin |
| Depth of cut follows the original chart's rules: slotting at 1×D radial, profiling at 0.35×D radial, both at 1×D axial. Feed per revolution was linearly interpolated from the chart's .078/.093/.125/.187/.250 inch columns. Note that the chip load in Harvey's chart is feed per revolution (IPR), not feed per tooth. | |||||
Feed falls between 510 and 800 mm/min. That means a 2,500 mm/min machine limit leaves more than 3x headroom; in CFRP work you will never be held back because "the machine can't go faster."
Required spindle speed rises steeply as tool diameter shrinks. A 6 mm tool needs only 5,000–6,500 rpm, while a 2 mm tool needs 14,500–19,400 rpm. The smaller the tool, the more it depends on the spindle's high-speed capability.
Tool diameter vs. required spindle speed, against the spindle limit
Required spindle speed for two fiber-content ranges, compared with a 20,000 rpm spindle limit
Stepping Down: Reduce Chip Load Beyond 1×D
Onsrud's composite cutting recommendations divide machining into three stages; the deeper the cut, the more the chip load must be reduced:
| Stage | Axial depth of cut | Chip-load adjustment | Actual depth with a 4 mm tool | Typical use |
|---|---|---|---|---|
| Finishing | 1 × D | Use recommended value | 4 mm | Final profile; finishing pass after leaving 0.1–0.2mm stock |
| Semi-finishing | 2 × D | Reduce 25% | 8 mm | Medium-thick sheet in a single full-depth pass |
| Roughing | 3 × D | Reduce 50% | 12 mm | Slotting thick sheet, heavy material removal |
| Onsrud's recommended starting speeds: 10,000–12,000 rpm for 1/8–3/16″ (3.2–4.8mm) and 8,000–10,000 rpm for 1/4″ (6.35mm); PCD tools generally 12,000–16,000 rpm. This is consistent in direction with the Harvey conversions in the table above. | ||||
Typical frame plates are 2–3mm thick and arms 5–6mm. Cutting 3mm sheet with a 4 mm tool, the 3mm depth of cut is less than 1×D, which falls in the "finishing" range: you can go full depth in one pass at the recommended chip load. For a 6mm arm, 6mm = 1.5×D, which falls in the semi-finishing range, so reduce the chip load, or simply split it into two 3mm passes.
Thermal Thresholds: 120°C Is the Red Line, 80°C the Sweet Spot
Heat dissipation is the most common concern about dry machining, and there is experimental data on it. A 2012 study by Pecat, Rentsch, and Brinksmeier found that subsurface thermal damage begins when the workpiece reaches 120°C, while machining results are best at about 80°C (close to the glass transition temperature of the epoxy). The same study also found a problem in the other direction: cracking was frequent at workpiece temperatures between −40°C and 20°C, and moderate warming actually prevented it.
But high spindle speed does not necessarily cause overheating. A 2013 study by Yashiro et al. showed that under dry down-milling conditions, cutting speeds can reach 300 m/min without exceeding the glass transition temperature of the matrix. In other words, temperature depends not only on spindle speed but also on chip evacuation, load per tooth, and tool sharpness.
| Workpiece temperature | Result | Corresponding parameter condition |
|---|---|---|
| −40 to 20 °C | Frequent cracking | Environment too cold; material more brittle |
| About 80 °C | Best machining results | Typical operating point with normal parameters and chip evacuation |
| 120 °C and above | Subsurface thermal damage | Dull tool, excessive depth of cut, or poor chip evacuation |
| Per Pecat, Rentsch & Brinksmeier (2012), Procedia CIRP 1:466-470. Temperatures are workpiece temperatures, not instantaneous cutting-edge temperatures. | ||
Climb or Conventional Milling? The Literature Is Split
This is the most hotly argued question online, but its real impact ranks far down the list. Here is what the literature says:
| Position | Conclusion | Source |
|---|---|---|
| Favors conventional | The best quality in trimming GFRP and CFRP is achieved with conventional milling, regardless of tool geometry and cutting conditions | König et al. (1985), Annals of the CIRP |
| Favors conventional | Conventional milling gives a better surface than climb milling; delamination was observed with climb milling | López de Lacalle et al. (2009) |
| Favors conventional | Tests with diamond interlocking-tooth tools: less delamination with conventional than climb milling, and feed rate matters more than spindle speed | Janardhan et al. (2006), SAE |
| Favors climb | Climb milling helps evacuate dust, while conventional milling presses dust into the surface layer; in climb milling the edge can cool in the air | Müller-Hummel et al. (2010), SME |
Most of the literature favors conventional milling for better edge quality, but the arguments for climb milling (dust evacuation and tool temperature) matter just as much in dry machining. The pragmatic advice: if edge quality comes first, use conventional milling; if dust evacuation and tool life come first, use climb milling. And before you agonize over this, make sure the tool is sharp and the depth of cut is reasonable; that pays off far more than the choice of milling direction.
A Trade-Off You Must Know: Quality and Dust Pull in Opposite Directions
Measurements by Dvořáčková et al., published in Polymers in 2024, found that the smallest dust particles (1.7 µm) occurred at "a low cutting speed of 120 m/min + a high feed per tooth of 0.2 mm/tooth". In other words, the "low speed, high feed" you might choose to protect the tool and save time produces exactly the fine particle size that is most hazardous to the lungs.
Conversely, high speed and low feed are kinder to both surface quality and particle size, but the total amount of dust generated per unit time does not go down. Whichever parameter set you use, dust collection and respiratory protection are not optional.
Practical Starting Parameters: Where to Begin Tuning
Here is all of the data above condensed into a starting point you can put straight on the machine. The example is the most common case: 3mm 3K carbon fiber sheet with a 4 mm diamond-coated multi-flute end mill.
| Parameter | Starting value | If edges fray | If the tool overheats | If the workpiece vibrates |
|---|---|---|---|---|
| Spindle speed | 9,000 rpm | Raise to 12,000 | Lower to 7,000 | Keep |
| Feed rate | 600 mm/min | Lower to 450 | Raise to 750 | Lower to 400 |
| Axial depth of cut | 3 mm (full depth in one pass) | Two passes of 1.5mm | Two passes of 1.5mm | Three passes of 1mm |
| Radial depth of cut | 1.4 mm (0.35×D) | Lower to 1.0 | Keep | Lower to 0.8 |
| Milling direction | Conventional | Stay conventional | Switch to climb (better dust evacuation) | Keep |
| Other | — | First check whether the tool is dull | Check whether dust collection is clogged | Check workholding |
| Starting values are taken from the middle of the 4 mm profiling range in this article's Harvey Tool conversion table. Change only one parameter at a time and record the result; otherwise you cannot tell which variable caused the improvement. | ||||
When edges start to fray, most people's first move is to adjust parameters. But in reality the most common cause is a tool that has already gone dull. Harvey Performance's technical documentation states plainly that once a tool starts to dull, cut quality drops quickly, and that CFRP calls for preventive tool changes rather than waiting for visible signs of wear. Put in a new tool and make a test cut first, then decide whether to touch the parameters. That order saves a great deal of wasted trial and error.
FAQ
Why do tool makers give feed per revolution instead of feed per tooth?
Because multi-flute end mills made for composites (burr end mills, staggered-tooth burrs) have many flutes and irregular edge shapes, so calculating with feed per tooth gives misleading results. Onsrud even notes that some series should be "treated as a single flute" for feed calculations. In practice, multiply feed per revolution by spindle speed to get mm/min, and do not multiply by the flute count again.
Should edges running in different directions on the same sheet get different parameters?
In theory, yes, because the fiber cutting angle θ changes with direction, and cutting forces at 0° and 90° differ noticeably (Elgnemi et al. 2021 found surface damage worst at 45° and 90°). In practice, though, a single profile toolpath passes through every angle anyway, so changing speeds segment by segment has limited benefit. A more effective approach is to use conservative parameters overall and leave a finishing allowance in the known critical directions.
If I can't use all of 2,500 mm/min, is there any point in buying a machine with a higher feed rate?
Not for pure CFRP work. But if you also cut thermoplastic sheet such as ABS, PMMA, or PC, the picture changes: reasonable feeds for those materials can reach several thousand mm/min, and that is when the feed limit becomes the bottleneck. When choosing a machine, look at your actual mix of materials, not just carbon fiber.
What happens if my spindle can't reach the tool maker's recommended speed?
The actual cutting speed will be lower than recommended, outside the tool's designed sweet spot. The usual result is higher cutting forces, fibers that are more likely to be pushed aside than cut, and poorer edge quality. To compensate, lower the feed at the same time to keep feed per revolution close to the target, and switch to a larger-diameter tool so the required spindle speed falls back within reach.
Do these parameters also apply to GFRP and FR4?
Harvey Tool's datasheet already lists "Carbon/Glass Fiber" together, so GFRP can use the same ranges. FR4 is a glass-fiber epoxy laminate and cuts much like GFRP, but note that FR4 dust contains glass fiber, so the protection requirements differ from carbon fiber. Before running real parts, we still recommend a test cut on scrap.
Sources
- Harvey Tool, Speeds & Feeds — End Mills for Composites, Diamond Cut (Series 6989xx / 7852xx, SFM and chip load chart), accessed September 3, 2026 — https://harveyperformance.widen.net/content/lp2peneiuc/original/SF_785200.pdf
- Onsrud, Composite Cutting Data Recommendations (depth-of-cut stages, chip-load adjustment, and starting speeds), accessed September 3, 2026 — https://onsrud.com/images/Composite.pdf
- Harvey Performance, CFRP Machining Tips (CFRP fails by brittle fracture rather than forming continuous chips; preventive tool changes), accessed September 3, 2026 — https://www.harveyperformance.com/in-the-loupe/cfrp-machining-tips/
- Hintze, Hartmann & Schütte (2011), Occurrence and propagation of delamination during the machining of CFRP, Composites Science and Technology (fiber cutting angle θ and the critical cutting zone) — https://doi.org/10.1016/j.compscitech.2011.08.002
- Pecat, Rentsch & Brinksmeier (2012), Influence of milling process parameters on the surface integrity of CFRP, Procedia CIRP 1:466-470 (120°C thermal damage threshold, 80°C optimum) — https://doi.org/10.1016/j.procir.2012.04.083
- König, Wulf, Graß & Willerscheid (1985), Machining of fibre reinforced plastics, Annals of the CIRP 34/2:537-548 (better quality with conventional milling)
- Janardhan, Sheikh-Ahmad & Cheraghi (2006), Edge trimming of CFRP with diamond interlocking tools, SAE 2006-01-3173 (feed rate matters more than spindle speed)
- Dvořáčková, Kroisová, Knápek & Váňa (2024), Polymers 16(18):2559 (particle size distribution of CFRP milling dust vs. parameters) — https://doi.org/10.3390/polym16182559
- Abena, Soo, Ataya et al. (2023), Chip Formation and Orthogonal Cutting Optimisation of Unidirectional Carbon Fibre Composites, Polymers 15(8):1897 (damage depth at each fiber angle) — https://pmc.ncbi.nlm.nih.gov/articles/PMC10144788/
- Wang et al. (2017), Study on Damage Evaluation and Machinability of UD-CFRP for the Orthogonal Cutting Operation, Materials 10(2):204 (damage factor measured by scanning acoustic microscopy) — https://pmc.ncbi.nlm.nih.gov/articles/PMC5459173/
- Hintze & Hartmann (2013), Modeling of Delamination During Milling of Unidirectional CFRP, Procedia CIRP 8:444-449 (initial boundary-layer damage depth vs. fiber cutting angle) — https://d-nb.info/1181855705/34
- Carbon-CNC Carbon Pro / Carbon Lite machine specifications (spindle 20,000 rpm, feed max. 2,500 mm/min) — https://www.carbon-cnc.com/en/carbon-pro/
The Right Parameters Need a Spindle That Can Run Them
Carbon-CNC's BLDC brushless spindle is adjustable up to 20,000 rpm, covering the full parameter range for 2 mm to 6 mm tools on structural CFRP. To discuss starting parameters for your sheet materials and parts, contact us.
Get a Quote