Worms - Coordinate Systems and Safety

Coordinate Systems, Machine Zero & Safety (Mazak EIA/ISO & Siemens Sinumerik)

The EvoSpline NC Generator outputs pure ISO/DIN G-code (EIA/ISO for Mazak and DIN 66025 for Siemens Sinumerik). If you are accustomed to conversational programming systems such as Mazatrol or ShopTurn, pay close attention to how coordinate systems, tool change positions, thread directions, and unit systems are handled in raw G-code.

1. Workpiece Coordinate System (WCS) & Z-Axis Polarity

In standard CNC turning, all coordinates positioned behind the part face (toward the chuck/spindle) carry a negative sign (-).

Z = 0: Typically set at the finished front face of the workpiece.
Z-Start & Z-End: Define the working range along the Z-axis (e.g., Z-start: 2.00 mm, Z-end: -65.00 mm).

2. Thread Direction Verification (Worm Hand: RH vs. LH)

Before generating code, check the live Worm hand indicator in the software.

EvoSpline automatically calculates whether the worm will be Right-Hand (RH) or Left-Hand (LH) by analyzing two parameters simultaneously:

Z-axis movement direction: Cutting towards the chuck (Z-Start > Z-End) vs. cutting towards the tailstock (Z-Start < Z-End).
Spindle rotation: Clockwise (M3) vs. Counter-Clockwise (M4).

⚠ Operator Tip: Always verify that the calculated Worm hand matches your engineering drawing before running the cycle on the machine.

3. Tool Change Positions in Absolute Machine Coordinates

The Tool change pos X and Tool change pos Z fields define the safe coordinates where the turret moves at two critical moments:

Program Start: The machine indexes to the chosen tool at this position before approaching the workpiece.
Program End: After the threading passes are complete, the turret returns here to allow safe part inspection, deburring, or unloading.

Control-Specific Retract Behavior:

Mazak (EIA/ISO) – G53 Logic:
EvoSpline outputs tool change moves using the G53 command (Machine Coordinate System).
These values are completely independent of your active workpiece zero (G54, G55, etc.). Even if you shift the part zero 200 mm deeper toward the chuck, the turret will always stop at the exact same physical machine location.
Siemens Sinumerik – SUPA and D0 Logic:
On Sinumerik controls, EvoSpline generates: SUPA G0 X... D0 SUPA G0 Z... D0

SUPA suppresses all settable zero offsets (G54–G599), frame shifts, and tool offsets for that specific block.
D0 explicitly deselects the active cutting edge offset during retract. This guarantees that the turret retracts to a fixed, safe machine coordinate regardless of active tool length geometry or workpiece zero shifts.

💡 Machine Coordinates Reference:

If you are unsure of your machine’s reference limits, enter 0 (often a safe reference limit, especially on X). Alternatively, jog the lathe manually to a clear, safe tool change position, read the machine coordinates directly from the CNC position display, and input them into EvoSpline.

4. Retract Distance (Clearance)

The Retract distance defines how far the tool pulls back in the X-axis before rapid traversing back to Z-Start for the next pass.

Ensure this value provides sufficient radial clearance from the outside diameter of the part, chuck jaws, and tailstock body.

5. Units of Measurement & Control Preparatory G-Codes

CNC controls interpret imperial and metric modes using different preparatory codes. Running a program with mismatched units will cause axis scaling errors or severe tool collisions.

Control System	Metric Mode (mm)	Imperial Mode (inch)
Mazak (EIA/ISO)	`G21`	`G20`
Siemens Sinumerik	`G71`	`G70`

⚠ Important: Always verify that your lathe is pre-configured or switched to the matching measurement system (G20/G21 for Mazak, G70/G71 for Sinumerik) before executing the cycle.

Worms Module (Metric): Generates all coordinates, feeds, and thread pitches in millimeters (mm).

Worms Module (Imperial): Generates all dimensions, tool geometry, and feeds in inches (in).

<< Previous

Next >>