HelixFeed

HelixFeed User Guide

Getting Started

HelixFeed reads your Fusion 360 CAM operations and recommends feeds, speeds, and cut geometry based on your material, tooling, and machine. Basic workflow:

• Select your material family and alloy
• Set your machine limits and rigidity (do this once, save it in your head)
• Review the calculated numbers for each operation
• Adjust intensity or override DOC/WOC if needed
• Check the boxes on the ops you want to update and hit Apply
• Regenerate toolpaths in Fusion as usual

Material & Alloy

Pick a family first (e.g. Aluminum, Steel, Stainless), then the specific alloy. If your alloy isn't listed, pick the closest equivalent — same temper and hardness range matter more than the exact grade number. 6061-T6 and 6082-T6 behave nearly identically, for example.

Intensity

Think of it as a throttle. 0% is a conservative finish pass. 100% is the full calculated chip load — as aggressive as the math says the tool and material can handle. 50% is a reasonable starting point on an unknown setup.

The global slider sets the default for all operations. Each operation has its own slider to override that default. Use per-op intensity to rougher-first, finish-last without touching the global setting.

Machine Settings

• HP Limit — Your machine's spindle horsepower. HelixFeed will back off chip load if the calculated power demand exceeds this. When it kicks in, you'll see the HP LIM badge.
• RPM Limit — Your spindle's top speed. Results will be capped here. Small-diameter tools on slow machines will show the RPM CAP badge.
• Max Torque — In in-lb. Set if your spindle has a low-speed torque limit (common on belt-drive machines and some VMCs). Leave blank if not applicable.
• Min RPM — Some machines won't hold speed well below a threshold. Set this and HelixFeed won't recommend lower. Leave blank if not applicable.
• Max Feed Rate — Machine's physical rapid or feed limit in IPM (or mm/min in metric mode). Set this if your machine can't keep up with calculated feeds. Leave blank if not applicable.

Machine Rigidity

This slider scales the aggressiveness of the recommendations to match how solid your machine actually is. It is the single most important calibration step.

Preset ranges as a starting point:

• 0.20 – 0.35 — Desktop / hobby (Sherline, Taig, benchtop mills)
• 0.36 – 0.54 — Light-duty (Tormach 440, mini VMC, older knee mills)
• 0.55 – 0.74 — Mid-range VMC (Tormach 1100, HAAS Mini Mill, small Brother)
• 0.75 – 0.89 — Full-size VMC (HAAS VF-2/VF-4, Mazak, Fanuc-driven 40-taper)
• 0.90 – 1.00 — Production VMC / HMC (heavy 50-taper, twin-pallet, high-pressure through-coolant)

To calibrate your machine: open a program you've already dialed in and are happy with. Run HelixFeed on the same material and tool. Adjust the rigidity slider until HelixFeed's numbers match what you're actually running. That's your machine's number — set it and leave it.

Workholding

Set per setup (per vise or fixture group). It applies an additional scale on top of machine rigidity to account for how well the part is held.

• Solid Fixture — Hard jaw, dowel-pinned fixture, zero-point system. Full rigidity.
• Standard Vise — Normal parallel-jaw vise, well-supported. Default.
• Soft Jaws / Toe Clamps — Some compliance. Dial back slightly.
• Tall Part / Thin Wall — Significant chatter risk. Use this for anything tall relative to its footprint, thin-walled pockets, or parts prone to ringing.
• Minimal Holding — Part is barely held in, or you're cutting near the jaw line. Very conservative.

Reading Your Results

• RPM — Spindle speed, already capped to your RPM Limit.
• Feed (IPM) — Cutting feed rate. This is what goes into Fusion's feed field.
• DOC — Depth of cut (axial). Stepdown in Fusion terms.
• WOC — Width of cut (radial). Stepover in Fusion terms.
• SFM — Surface feet per minute. Shows where you are relative to the tool's ideal cutting speed for this material.
• IPT — Inches per tooth. This is your chip load — the metric most tool manufacturers give limits for.
• Plunge — Plunge feed rate. Applied to ramp and plunge moves in the toolpath.
• MRR — Material removal rate in cubic inches per minute. Useful for comparing strategies.
• HP Required — Estimated spindle draw at these parameters. Compare to your HP Limit.
• Coolant — Recommended coolant strategy (Flood, Mist, Air Blast, Dry) based on material.

Machining Modes

• Auto — HelixFeed picks the best mode based on the Fusion operation type. Use this by default.
• Roughing — Conventional full-width cuts. Higher chip load, deeper DOC, higher MRR.
• Adaptive Roughing — Constant-engagement toolpath (Fusion Adaptive). Light WOC, full DOC, high feed. Maximizes MRR and tool life.
• Wall Finish — Light WOC, full LOC, lower chip load. For finishing vertical walls to final dimension.
• Floor Finish — Very light DOC, moderate WOC. For finishing horizontal floors.
• Slotting — Full-width engagement. Chip load backed off heavily — slotting is brutal on tools. Increase feeds from here with caution.
• Surface Finish — Ball-end finishing passes. Chip load and stepover driven by the cusp height target.

Safe Mode

Forces the operation to 25% intensity with automatic geometry (no Full LOC). Use it on any operation where you're unsure about tool condition, setup, or material behavior. It's a one-click conservative preset — not a permanent mode. Disable it when you're confident in the numbers.

Full LOC (Length of Cut)

Full LOC means HelixFeed uses the entire tool's flute length as the axial depth of cut, with a proportionally lighter radial engagement. This is the basis of High Efficiency Machining (HEM) and trochoidal strategies — deep axial, narrow radial, constant engagement. It distributes heat and wear across the whole flute instead of just the tip.

When to use it: adaptive roughing, wall finishing, any time you're running a long-reach tool or want to maximize tool life. Slotting and floor finishing force Full LOC off automatically since it doesn't apply to those cut geometries.

Overrides

The DOC (Stepdown) and WOC (Stepover) fields under each operation let you pin a specific value rather than using the calculated one. The field shows the calculated value as a placeholder — type in your own to override. Hit the reset link next to the label to go back to auto. Overrides survive recalculation until you reset them.

Warning Badges

• HP LIM — Feed rate or chip load was reduced because the calculated HP exceeded your limit.
• RPM CAP — Spindle speed hit your RPM Limit. SFM will be lower than ideal — consider a smaller tool if available.
• ANTI-RUB — RPM was floored to avoid rubbing (too slow for the material). Occurs when RPM would otherwise fall below the minimum SFM threshold.
• TORQUE LIM — Feed reduced because spindle torque at this RPM would exceed your Max Torque setting.
• SHAFT RISK — The tool shank is estimated to be near its torsional limit. Reduce intensity, reduce DOC, or use a shorter-reach tool. Take this one seriously.
• Machine rigidity pill — Shows the effective rigidity factor after combining machine and workholding. Turns yellow when the floor (minimum safe engagement) is the binding constraint.
• Feed capped — Max Feed Rate setting limited the output. RPM was also adjusted to protect chip load at the capped feed.

Applying to Fusion

Check the boxes on the operations you want to update, then click Apply Feeds & Speeds. HelixFeed writes the calculated values into those Fusion operations — RPM, feed rate, plunge rate, stepdown, and stepover.

Apply does not run the toolpath. You still need to regenerate operations in Fusion (right-click > Generate, or use the Generate All button) before posting code or simulating. If you have Auto-generate checked in Machine Settings, Fusion will attempt to regenerate immediately after apply — useful for quick previews, but disable it for large setups.