Turning Parameters

Machining Mode

Workpiece Orientation

Blank Diameter (X)

Target Diameter (X)

Turned Length (Z)

Depth of Cut (MID / ap)

Finishing Allow. X (FALX)

Finishing Allow. Z (FALZ)

Front Edge Feature

Include Face-Off Pass

Spindle Mode

Cutting Speed (S)

m/min

Max Spindle Speed (LIMS)

RPM

Roughing Feed (FF1)

mm/r

Active offset

The program calls D1. CYCLE95 reads tool nose radius and orientation from that offset.

Profile Geometry Shape

CYCLE95 feeds & chip control

Plunge feed (FF2)

mm/r

Finishing feed (FF3)

mm/r

Chip dwell (DT)

Chip path (DAM)

Contour lift-off (_VRT)

MID and _VRT are positive radius values. Confirm the cycle settings used by your control software version.

Live Path Visualizer & Sinumerik Program

Configure turning parameters on the left and click Generate Sinumerik Program to initialize the live toolpath simulator and G-code export.

Add Tool to Offset Setup

Quick Preset Lathe Tools

+ CNMG 120408 (Rougher) + DNMG 150404 (Finisher) + Parting Blade 3mm + Thread Chaser 60° + U-Drill Ø20 + Boring Bar CCMT

Tool number & name

Must begin with the numeric T data record used by your control.

Active Edge (D)

Siemens Tool Type Code

Length 1 (X Geometry)

Length 2 (Z Geometry)

Tool Nose Radius (R)

Cutting Edge Position

Click Cutting Edge Quadrant (Type 1-9)

Wear X (ΔX)

Wear Z (ΔZ)

Sinumerik Tool Offset Table

No tools added to the offset setup card yet. Fill in offsets on the left or click a Quick Preset.

The .TOA export uses the numeric part of each T identifier as the Sinumerik tool data-record number. Confirm the record and edge numbers against the target control before importing.

SHADER7 SINUMERIK SETUP CARD

PROGRAM: SH7_TURNING_CYCLE.MPF DATE: CONTROL: SIEMENS 840D / 828D

Tool ID	Edge (D)	Type	Length X (L1)	Length Z (L2)	Radius (R)	Point Dir	Wear X	Wear Z
No tools loaded in setup.

Ensure tool nose radius compensation (G41/G42) is calibrated prior to executing CYCLE95 programs. Always verify clearances on first dry run.

Turning Speeds, Feeds & Power Calculator

Estimate spindle RPM (\(n\)), axial feed rate, material removal rate, and theoretical surface finish (\(Ra\)) for Siemens turning programs.

Material Preset

Cutting Diameter (D)

Cutting Speed (Vc)

m/min

Feed Rate (f)

mm/r

Depth of Cut (ap)

Tool Nose Radius (rε)

Calculated Spindle Speed 1061 RPM n = (Vc × 1000) / (π × D)

Axial Feed Rate 265 mm/min Vf = n × f

Material Removal Rate (MRR) 100 cm³/min Q = Vc × ap × f

Surface Roughness Ra / Rz 2.44 / 9.77 µm Ra ≈ f²/(32rε) | Rz ≈ 4×Ra

Welcome to the Sinumerik G-Code Suite

Siemens Sinumerik controls (including the 840D, 828D, and 808D) utilize a sophisticated, high-level CNC programming language. Unlike ISO standard G-code (Fanuc/Haas), Siemens supports named variables, parameterizable canned cycles, local contour labels, and advanced tool management. This suite provides professional shop-floor tools to write correct Siemens turning code and generate standardized offset setup cards.

G-Code Turning Fundamentals

Turning on Siemens systems is programmed in the G18 Z-X plane. Key preparatory commands:

Command	Description
`G18`	Select ZX Plane (Standard for Lathes)
`G95`	Feed per Revolution (e.g. F0.25 = 0.25 mm/rev)
`G96`	Constant Surface Speed (CSS in m/min)
`LIMS=...`	Spindle RPM Clamping Limit during G96
`G97`	Constant Spindle Speed (Direct RPM)
`DIAMON`	Diameter programming active for X axis
`G41 / G42`	Tool nose radius compensation Left / Right
`G40`	Cancel tool nose radius compensation

Cycles Sinumerik Lathe Cycles

Siemens uses built-in parameterizable canned cycles for automated machining:

Cycle	Operation Description
`CYCLE95`	Stock Removal / Contour Roughing & Finishing
`CYCLE93`	Grooving & Part-off Cycle
`CYCLE97`	Thread Cutting (Metric, Whitworth, API)
`CYCLE98`	Thread Chain (Continuous threads)
`CYCLE83`	Deep Hole Drilling with Peck & Chip Break
`CYCLE84`	Rigid Tapping without Floating Chuck

CYCLE95 Parameter Reference Breakdown

Syntax: CYCLE95(NPP, MID, FALZ, FALX, FAL, FF1, FF2, FF3, VARI, DT, DAM, _VRT)

Parameter	Name	Explanation & Values
`NPP`	Contour Name	Contour subprogram name or an inline label range. Generated programs use `"CONTOUR_START:CONTOUR_END"` so the MPF stays self-contained.
`MID`	Infeed Depth	Maximum depth of cut per pass along radius (\(a_p\)), programmed as positive number.
`FALZ / FALX`	Finishing Allowance	Finishing allowance on longitudinal axis Z (FALZ) and diameter axis X (FALX).
`FF1`	Roughing Feed	Feedrate for roughing passes along parallel contour lines.
`FF2`	Plunge Feed	Feedrate for downward plunge moves into undercut contours.
`FF3`	Finishing Feed	Feedrate for the final contour-following finishing cut.
`VARI`	Machining Type	1–4 rough: longitudinal external, face external, longitudinal internal, face internal. 5–8 finish: the same four orientations. 9–12 complete: the same four orientations. This generator uses 1/3, 5/7 and 9/11 for longitudinal OD/ID.

Compare Sinumerik vs. Fanuc Lathe

Feature	Siemens Sinumerik	Fanuc / ISO
Tool Call	`T="ROUGH" D1` or `T1 D1`	`T0101`
CSS Clamp	`G96 S200 LIMS=3000`	`G50 S3000`
Rough Cycle	`CYCLE95(...)`	`G71 U... R... / G71 P... Q...`
Thread Cycle	`CYCLE97(...)`	`G76 P... Q... R...`
Contour End	`M17`	`M99`

Types 1-9 Cutting Edge Position (T Position)

Specifies the quadrant position of the tool nose relative to the holder center for G41/G42 tool nose compensation:

Type	Orientation Description	Common Tool
`Type 3`	Points Left & Up (Quadrant 3)	Standard OD Right-Hand Turning
`Type 2`	Points Left & Down (Quadrant 2)	Boring Bar (ID Turning)
`Type 1`	Points Right & Up (Quadrant 1)	Back Turning / Reverse OD
`Type 7 / 8`	Straight Face / OD Grooving	Parting / Grooving Insert
`Type 9`	Theoretical Tool Center	Drills, Center Drills, Taps