CNC Turning Profiles and Cycles

A rounded tool nose does not cut at the imaginary sharp tip

A turning insert has a rounded corner, called its nose radius. Touching off along X and Z establishes an imaginary tip: the intersection of the two tangent reference lines. There is no cutting material at that intersection. The actual contact point moves around the nose as the direction of the surface changes.

Axis-parallel cuts can reach the measured diameter or face with the corresponding touch-offs. On a taper, chamfer or arc, simply driving the imaginary tip along the desired surface leaves a profile error. Account for the nose radius with a calculated toolpath or the control's tool nose compensation. See Turning Tapers for taper geometry.

Compensation needs nose radius, tip orientation and a clear entry and exit

In common Fanuc-style usage, G41 selects compensation to the left of the programmed direction of travel and G42 to the right; G40 cancels it. Judge the side in the control's XZ-plane convention. Do not choose a code from the screen's apparent left or right, or assume one code means every outside cut.

Enter the actual nose radius and the control's tip orientation, which tells it where the imaginary tip sits relative to the nose centre. Select the correct tool-offset register, use the manual's lead-in and lead-out requirements, and check the resulting path with CNC Programming and Prove-Out. Tip numbers differ by control; there is no universal number table here.

Do not apply full nose-radius compensation again to a path already corrected for that radius. Check whether a CAM post expects full geometry compensation, wear-only compensation or no control compensation.

A roughing cycle removes layers while leaving stock for finishing

A G71-type roughing cycle uses a defined final profile to generate repeated stock-removal passes, commonly along Z for outside or inside turning. The programmer supplies the applicable cut depth, retract and finish allowance. A G70-type finishing cycle follows the defined profile to remove the remaining allowance.

Read the control's cycle definition before entering parameters. One-block and two-block formats differ. A depth word may be radial while an X allowance is diametral; the same letter can mean different things in different blocks. P and Q commonly identify the first and last numbered profile blocks. Check the referenced blocks, permitted profile direction changes, return path and compensation rules.

Grooving repeats plunges; threading synchronizes feed with rotation

A grooving or peck cycle divides a plunge into smaller advances and retracts. Some formats repeat the plunge at different Z positions to make a wider groove. G75 is one common outside/inside grooving family; face-grooving and peck-drilling families may use other codes. Check peck size, final depth, groove width and tool-width convention separately.

A G76-type threading cycle makes repeated synchronized passes with increasing depth. The thread lead determines the axial advance per spindle revolution. The cycle also needs control-specific information about final size, infeed, pass depth and runout. Use Single-Point Threading for pitch, lead and thread form; a threading cycle does not choose those dimensions for you.

Formats differ by control, so no complete parameter syntax is universal. See the Haas G75 reference and the G70/G76 entries in its lathe workbook as examples. CNC Turning Program Walkthrough spells out ordinary moves so the sequence can be read without decoding a cycle.