Each row in the Cutting Parameters Explorer is a measure of the cut: how deep and wide it is, how fast it runs, and how hard it loads the tool, spindle and workholding. Some rows you can limit; others are read-outs that change as you move the rest. This article explains what each measure means, why it matters, and which ones you'll see for each kind of operation.
For how to open the explorer and use its controls, see The Cutting Parameters Explorer.
Adjustable rows and read-outs
- Adjustable rows have range handles. Drag them to limit the measure, reset it, or lock it to type an exact value. CAM Assist then finds cutting parameters that stay inside your limits.
- Read-outs are for information only. They update as you change other rows, but you can't set them directly.
These measures are always read-outs, marked Result only: Material removal rate, Maximum geometric cusp size, Feed per tooth, Plunge feed rate, Ramp feed rate and Step down. Any other row is adjustable when CAM Assist has a recommended range for it in that operation, and greyed out when it doesn't.
Units follow your unit setting. The units below are metric. See Switch between mm and inches in CAM Assist.
Engagement: how much the tool cuts
| Measure | Unit | What it means | Why it matters |
|---|---|---|---|
| Depth of cut (Ap) | mm | How far the tool engages along its own axis on each pass. | The biggest lever on how much material each pass removes. Deeper cuts are faster but raise cutting force, heat and deflection. Too deep gives chatter, a poor finish or a broken tool. |
| Width of cut (Ae) | mm | How much of the tool's diameter engages sideways (the step over in roughing). | Works with depth of cut to set the load. Wider is faster but pushes harder on the tool and the part. |
| Step over | mm | Distance between neighboring finishing passes, measured across the surface. | Smaller step over leaves smaller cusps and a better finish, but takes more passes. |
| Step down | mm | Vertical distance between passes as the tool works down a surface. Read-out. | Shows how finely the surface is covered in height. |
| Stock to leave | mm | Material deliberately left on the surface by this operation. | Leaves material for a later operation to finish to size. |
| Tool approach direction | degrees | The angle at which the tool meets the surface on a freeform pass. | Lets you control how the tool meets the surface on freeform finishing. |
| Offset tip to feature | mm | How far the chamfer tool's tip sits below the edge it's cutting. | Sets where the chamfer is cut on the tool's angled edge. In a preset this is Min tip offset. |
Speeds and feeds
| Measure | Unit | What it means | Why it matters |
|---|---|---|---|
| Spindle speed | rpm | How fast the spindle turns. | Comes from the surface speed and the tool diameter. Limit it if your machine has a speed it can't exceed or runs best at. |
| Surface speed | m/min | How fast the cutting edge moves past the material (cutting speed, Vc). | The main driver of cutting heat and tool life. It depends on the material and the tool. |
| Feed rate | mm/min | How fast the tool travels through the material (table feed). | The speed you see on the machine. Faster feeds finish sooner but raise cutting force, heat and tool load. |
| Feed per tooth | mm/tooth | How far the tool advances for each cutting edge that passes. Read-out. | Too low and the edges rub instead of cutting, wearing the tool. Too high and they overload. |
| Chip Load | mm | The thickness of the chip each cutting edge actually removes. | Drives tool life, heat and finish. Limit it if you have a preferred chip load for your tooling. |
| Plunge feed per rev | mm/rev | How far the tool advances into the hole for each revolution. | The main feed setting for drilling. Too little and the drill rubs and overheats; too much overloads the tip or packs the flutes with chips. |
| Plunge feed rate | mm/min | The straight-line speed of the tool as it plunges. Read-out. | Shows the feed that results from the plunge feed per rev and the spindle speed. |
| Ramp feed rate | mm/min | The feed used on the angled or helical move into the material. Read-out. | Ramping in gently protects the tool from plunging straight into solid material. |
| Ramp angle | degrees | How steeply the tool descends as it ramps or helixes in. | Shallow angles are easier on the tool but take longer to reach depth. Steep angles load the tool tip more. |
| Bore diameter | mm | The diameter of the helical path the tool follows. | Sets the size of the bore the helix produces. |
How the speed and feed measures relate
| Relationship | Formula |
|---|---|
| Surface speed from spindle speed | Surface speed (m/min) = spindle speed (rpm) × π × tool diameter (mm) ÷ 1000 |
| Feed per tooth from feed rate | Feed per tooth = feed rate ÷ (spindle speed × number of cutting edges) |
| Plunge feed rate from plunge feed per rev | Plunge feed rate = plunge feed per rev × spindle speed |
| Material removal rate (milling) | Material removal rate (cm³/min) = feed rate (mm/min) × depth of cut (mm) × width of cut (mm) ÷ 1000 |
Feed per tooth and Chip Load are the same when the width of cut is half the tool diameter or more. With a narrower width of cut the chip gets thinner than the feed per tooth (radial chip thinning), so the chip load is smaller.
Load on the tool, spindle and workholding
| Measure | Unit | What it means | Why it matters |
|---|---|---|---|
| Tool deflection (mean) | µm | How far the tool tip is predicted to bend away from the cut, on average, under cutting force. | A bending tool cuts in the wrong place: tapered walls, lost accuracy and chatter. Limit it to protect accuracy, especially with long or slender tools. |
| Break point | % | How close the stress in the tool gets to its limit, as a percentage. | Your margin against breaking the tool. 100% is at the limit; keeping it lower trades a little speed for safety. |
| Workholding security | N | The sideways force the cut puts on the part and the workholding. | Too much force can pull the part out of the vise or fixture. Limit it for light clamping or awkward setups. See What is workholding security in CAM Assist? |
| Spindle power (mean) | kW | The average power the cut draws from the spindle. | Must stay within what your spindle can deliver. Lower it to keep heavy cuts within a smaller machine. |
| Spindle torque | N·m | The twisting force at the spindle. | Matters most for heavy cuts at low rpm, where torque, not power, is the limit. See What spindle torque and power should I enter for my machine? |
Results: productivity and finish
| Measure | Unit | What it means | Why it matters |
|---|---|---|---|
| Material removal rate | cm³/min | The volume of material the cut removes each minute. Read-out. | The headline productivity number for roughing. It rises as you make other settings more aggressive. |
| Maximum geometric cusp size | µm | The height of the ridges (cusps) left between neighboring passes. Read-out. | Predicts how smooth a finishing pass will be. Smaller cusps need more passes. |
| Surface roughness | µm (Ra) | The predicted finish of the cut surface, as an Ra value. | Lets you aim straight at a finish specification. Lower Ra is smoother but usually means lighter, slower cuts. |
Which measures each operation shows
Which rows appear depends on the operation and the tool. Operations that ramp into the material, such as adaptive roughing and pocketing, have a Cutting usage and a Ramping usage, each with its own rows. Switch between them at the top of the explorer.
| Operation | Typical tools | Measures shown |
|---|---|---|
| Face roughing | Face mills | Depth of cut, Width of cut, Tool deflection, Break point, Material removal rate, Workholding security, Feed per tooth, Chip Load, Feed rate, Surface speed, Spindle speed, Spindle power (mean), Spindle torque |
| Face finishing, Flat finishing, Wall finishing, Undercutting (T-slot) | Face mills, end mills, ball end mills, T-slot cutters | As face roughing, plus Maximum geometric cusp size and Surface roughness |
| Adaptive roughing | End mills | Cutting: as face roughing. Ramping: the same load and speed rows, plus Plunge feed rate, Ramp feed rate, Ramp angle and Bore diameter. |
| Pocketing | End mills | As adaptive roughing. The slot is the full width of the tool, so width of cut is set by the tool. |
| Freeform | Ball end mills | Step over, Step down, Tool approach direction, Stock to leave, Tool deflection, Break point, Material removal rate, Workholding security, Maximum geometric cusp size, Surface roughness, Feed per tooth, Chip Load, Feed rate, Surface speed, Spindle speed, Spindle power (mean), Spindle torque |
| Chamfering, Deburring | Chamfer mills | Depth of cut, Offset tip to feature, Tool deflection, Break point, Material removal rate, Workholding security, Maximum geometric cusp size, Surface roughness, Feed per tooth, Chip Load, Feed rate, Surface speed, Spindle speed, Spindle power (mean), Spindle torque |
| Helical boring | End mills, bull nose end mills | As face finishing, plus Ramp feed rate, Ramp angle and Bore diameter |
| Drilling, Spot drilling | Drills, spot drills | Surface speed, Spindle speed, Plunge feed per rev, Plunge feed rate, Material removal rate |
| Tapping | Taps | Surface speed, Spindle speed, Plunge feed per rev, Plunge feed rate. The thread pitch sets the feed, so the speeds are what you work with. |
What this means for you
- Start with the Conservative to Aggressive slider, then limit only the measures that matter for the job, such as Tool deflection for a long tool or Workholding security for a weak clamp.
- Watch the read-outs, such as Material removal rate and Maximum geometric cusp size, to see what each change costs or gains.
- To keep values you like for future parts, save them as a preset. See Save cutting parameters as a preset.