Turning calculations (user guide)

mfgparams calculates parameters for single-point-tool turning on a lathe, alongside drilling and milling. This page covers using it from the interactive text GUI; see Turning API reference (developers) for the library API.

Selecting an operation in the text GUI

Launch the text GUI with:

mfgparams

A persistent menu bar stays visible at the top of the screen: Exit, Machining, Configuration, About, Help. Selecting Machining expands a tree in place, showing Milling, Drilling, and Turning as flat leaves; selecting Turning opens its operation screen directly, with no further tree-level expansion. It appears as a centered, bordered floating window over the menu bar and tree (which stay visible underneath, untouched): the left pane lists every turning input at once (unit system, calculation mode, material type, material, turning tool, workpiece diameter, depth of cut, length of cut, available power), all simultaneously visible and editable; the right pane shows the live result, updating automatically as you fill in or change an input.

Up/Down (or j/k) always moves to the next/previous field, regardless of its type. A radio field (unit system, mode, material type, material, tool) is always a single Label: value line — Left/Right/h/l/ Space cycle its value with wraparound and commit it immediately. Once metal is chosen as the material type, the Material field also opens a dedicated selection window on Enter, on top of that ordinary cycling — see Selecting a metal material below. Numeric fields become editable the instant you select them; that text is only written to the field once you navigate away from it, exactly as described for drilling in Drilling calculations (user guide). Left/Right nudges the buffer up or down by a small step: workpiece diameter, depth of cut, and length of cut nudge by 1 mm under the metric unit system, or 0.1 in under the imperial unit system — a whole-inch step is too coarse for these dimensions — while available power nudges by the shared 1 display-unit step under either unit system.

Selecting a metal material

Once metal is chosen as the material type, the Material field still cycles one material at a time with Left/Right/h/l/Space, exactly like any other radio field — but pressing Enter on it instead opens a centered selection window for finding a material by more than just cycling through the list. It lists every metal material in three columns — common name, EN material number (e.g. 1.0038), and shortened/DIN-style designation (e.g. S235JR) — with an independent search field for each column; a material missing a recorded number/designation shows that cell blank. Tab/Right and Shift+Tab/Left switch which column’s search field receives typed characters, without losing text already typed into the others; typing narrows the list to materials matching every non-empty search across all three columns at once. Up/Down move the highlighted row; Enter selects the highlighted material and closes the window; Escape closes it without changing the current selection. Reopening the window always starts with the material you already had selected (if any) highlighted, and every search field cleared. This behaves identically to Drilling calculations (user guide)’s own Material field (same columns, search, navigation, and confirm/cancel keys) — see that page’s own “Selecting a metal material” section, or specs/023-material-selector-dialog/contracts/materials-config-schema-delta.md, for the materials-config schema that populates the extra two columns. Non-metal material types are unaffected and only ever offer the ordinary Left/Right/Space radio-cycling behavior, with no selection window.

Turning inputs

After the unit system, calculation mode, material type, material and tool, turning asks for three geometry values:

Prompt	Meaning
Workpiece diameter	Diameter of the workpiece being turned, in mm / in.
Depth of cut	Radial depth of material removed per pass, in mm / in.
Length of cut	Length of the turning pass along the workpiece, in mm / in.

The depth of cut must be strictly less than half the workpiece diameter (the workpiece radius) — a depth of cut at or beyond the radius is physically impossible and is rejected with a clear error rather than silently clamped.

Calculation modes

Turning supports six calculation modes: standard, power-constrained, and fixed-rpm behave identically to drilling’s — see Drilling calculations (user guide)’s “Calculation modes” section for the full description; only the geometry inputs above differ. Turning also has three turning-only modes:

feed-rate-constrained: instead of the feed rate per rotation being derived from the selected material and turning tool, you supply it directly — for example, to match a surface-finish requirement or a value already dialed into the lathe. Selecting this mode shows a required Feed rate per rotation field in place of the target-RPM field; spindle speed is still derived exactly as in standard mode (from the material’s and tool’s reference cutting speed and the entered diameter), but machining time, cutting force, torque, and power are all recomputed from your supplied feed rate instead of the material/tool’s reference value. In the text GUI, the Feed rate per rotation field nudges by a finer step than every other field when you press Left/Right: 0.1 mm/rev under the metric unit system, or 0.005 in/rev under imperial (finer than the geometry fields’ 0.1 in imperial step, and the 1 display-unit step available power uses).

rotation-and-feed-constrained: for when you already know both your exact spindle speed and your exact feed per rotation — for example, both are already dialed into the lathe. Selecting this mode shows required Target spindle speed and Feed rate per rotation fields together, plus an optional Available power field; neither the spindle speed nor the feed is derived from the material/tool — machining time, cutting force, torque, and power are all computed directly from the two values you supply. Because the spindle speed is entirely yours, the result panel labels it “user-specified,” the same as fixed-RPM mode’s.

power-and-feed-constrained: for when you know your available power budget and need a specific feed per rotation — for example, to meet a surface-finish requirement while staying within the lathe’s rated power. Selecting this mode shows required Feed rate per rotation and Available power fields (no spindle-speed field, since it is solved for rather than supplied); the module finds the highest spindle speed that keeps the operation within your power budget at your exact feed – but never above the cutting-speed-derived reference speed standard mode would use at that feed, so a generous budget still tops out at that reference speed rather than climbing further. The result panel labels spindle speed “adjusted to fit available power,” the same as power-constrained mode’s.

Reading the results

A turning result looks like this (40 mm diameter, 2 mm depth of cut, 100 mm length of cut, Mild Steel, Carbide, standard mode):

Spindle speed:     477.5 RPM    (recommended)
Feed rate:         100.3 mm/min
Feed per rotation: 0.21 mm/rev
Machining time:    1.00 min
Torque:            16.0 N·m
Power required:    0.80 kW
Cutting force:     798.0 N

Spindle speed and feed rate describe how the workpiece is turned, machining time is how long the pass takes, torque and power are what the spindle needs to deliver, and cutting force is the tangential force the tool experiences — the quantity a turning tool holder’s rated force is typically compared against. Feed per rotation expresses the same feed rate as an amount of material advance per workpiece rotation (mm/rev or in/rev) — the way feed rate is actually set on a lathe — alongside the existing per-minute feed rate, whose own meaning and value are unchanged. Turning does not report a material removal rate (that line is specific to milling) but is the only process that reports cutting force and feed per rotation, both of which stay None for drilling and milling results.

If you supply an available lathe/tool power and the calculated power exceeds it, the result is still shown, with a warning line telling you the cut is beyond what the machine can deliver.

Limits and validation

Workpiece diameter, depth of cut, and length of cut are each validated as part of the calculation itself: an out-of-range value produces a clear, actionable error in the right pane rather than a result. The bounds themselves are:

Setting	Default	Applies to
max_turning_diameter_mm	500.0 mm	Workpiece diameter.
max_turning_depth_of_cut_mm	10.0 mm	Depth of cut.
max_turning_length_of_cut_mm	1000.0 mm	Length of cut.

These are distinct from drilling’s and milling’s own bounds (e.g. max_depth_of_cut_mm, 50 mm) — a single-point turning tool’s realistic depth of cut per pass is far shallower than a milling cutter’s, so the two cannot share one bound. In addition, all three values must be positive, finite, and within their bound; NaN, +inf/-inf and non-numeric values are all rejected before the bound is checked, the same posture drilling and milling already apply (issue #56).

Library callers can override these bounds via calculate_turning()’s config_path argument (see Turning API reference (developers)).

Assumptions

The turning model uses standard single-point turning formulas as published in widely-referenced industry sources (Sandvik Coromant’s “Machining Formulas” reference and Machinery’s Handbook — the same class of source drilling’s own formulas cite). Unlike drilling, turning’s machining-time formula has no point-engagement allowance term, since a single-point turning tool has no drill-point geometry to account for. Only straight (outside-diameter) turning is in scope; facing, grooving, parting, threading, and taper turning are deliberately deferred to a later feature. See specs/019-turning-calculations/research.md for the formulas and their sources, specs/020-turning-feed-per-rotation/research.md for the feed-rate-constrained mode and feed-per-rotation reporting, and specs/021-turning-combined-constraints/research.md for the rotation-and-feed-constrained and power-and-feed-constrained modes.