MASSO Documentation

  1. Getting started - Wiring & Setting-up MASSO
  2. Warnings and Cautions
  3. Warranty
  4. MASSO Accessories
    1. Homing Sensor
    2. Optical Encoder
  5. Power On/Off Precautions
  6. Emergency Stop (E-Stop)
  7. Admin and User Passwords
  8. Graphical Interface
    1. Controller Alarms
  9. Touch Screen Interface
  10. Keyboard and Key Shortcuts
    1. Setting time
    2. Homing the machine
    3. Rapid/Jog
    4. MDI command
    5. Creating New G-Code Files
    6. Editing G-Code
    7. Resetting Job Counter
  11. Supported G & M-Codes
    1. G00 - Rapid Motion
    2. G01 - Linear Interpolation Motion
    3. G02 – Circular Interpolation (Clockwise)
    4. G03 – Circular Interpolation (Counter Clockwise)
    5. G04 – Dwell
    6. G10 – Set Work Offset Values
    7. G17 – XY Plane Selection
    8. G18 – ZX Plane Selection
    9. G19 – YZ Plane Selection
    10. G20 – Set Machine Units To Inches
    11. G21 – Set Machine Units To Millimetres
    12. G28 – Return To Machine Home
    13. G32 – Threading Cycle
    14. G38.2 – Straight Probe Cycle
    15. G53 – Move In Absolute Machine Coordinates
    16. G54 to G59 – Select Work Offset Coordinate System
    17. G73 – High Speed Peck Drilling
    18. G80 – Cancel Modal Motion
    19. G81 – Drilling Cycle
    20. G82 – Drilling Canned Cycle With Dwell
    21. G83 – Peck Drilling For Deeper Holes
    22. G90 – Set Distance Mode To Absolute
    23. G91 – Set Distance Mode To Incremental
    24. G92 – Temporary Work Offset
    25. G92.1 – Cancel Temporary Work Offset
    26. G93 – Inverse Time Mode
    27. G94 – Units Per Minute Mode
    28. G96 – Turn on Constant Surface Speed (CSS)
    29. G97 – Turn off Constant Surface Speed (CSS)
    30. G98 – Canned Cycle – Retract Back To The Initial Z
    31. G99 – Canned Cycle – Retract Back To R Plane
    32. M00 – Program Stop
    33. M01 – Optional Program Stop
    34. M02 – Program End
    35. M03 – Spindle ON (Clockwise)
    36. M03 – Plasma Torch ON
    37. M04 – Spindle ON (Counter Clockwise)
    38. M05 – Spindle OFF
    39. M05 – Plasma Torch OFF
    40. M06 – Tool Change
    41. M07 – Turn Mist Coolant On
    42. M08 – Turn Flood Coolant On
    43. M09 – To Turn All Coolant Off
    44. M10 – Chuck Or Rotary Table Clamp On
    45. M11 – Chuck Or Rotary Table Clamp Off
    46. M30 – End The Program And Rewind
    47. M62 – Turn On Digital Output Synchronized With Motion
    48. M63 – Turn Off Digital Output Synchronized With Motion
    49. M666 – Plasma – Turn THC Function Off
    50. M667 – Plasma – Turn THC Function On
    51. M98 & M99 – Sub Program Call
  12. Loading & Running G-Code
    1. Load File Menu
    2. Running G-Code Programs
    3. Stopping Program (Feed Hold)
    4. Resuming Program or Jump to Line
    5. Restarting Program from Start
    6. Auto Loading G-code
  13. Calibrating Tools
    1. Lathe Tool Calibration Steps
    2. Mill Tool Calibration Steps
  14. Work Offsets
  15. Conversational Programming
    1. Lathe Conversational Wizards
    2. Mill Conversational Wizards
  16. CAM Post Processors
    1. POST Processor Requirements
    2. Artcam
    3. BobCAD-CAM
    4. Fusion 360
    5. SheetCAM
    6. Vectric VCarve and Vectric Aspire
  17. Touch Probes & Plates
    1. Part Probing
    2. Automatic Tool Zero
    3. Touch Plate
  18. Wi-Fi Connectivity
  19. Mounting and Mechanical Data
  20. Setup and Calibration
    1. Power Connector
    2. Connecting Display
    3. E-Stop
    4. Door Input
    5. Save & Load Settings
    6. Setting default units to mm or inches
    7. Axis Calibration
    8. Axis Calibration Wizard
    9. Slave Axis
    10. Backlash Compensation
    11. Homing / Home Inputs
    12. Spindle Connector
    13. Spindle RPM Encoder
    14. List of Configurable Inputs
    15. List of Configurable Outputs
    16. TTL Outputs
    17. Relay Driver Outputs
    18. MPG Pendant
    19. Tower Lights
    20. Analog Inputs
    21. Serial Port
    22. PlayStation 2 Controller
    23. Replacing Optocouplers
    24. Installing or Replacing Backup Battery
  21. Motors & Drives Connections
    1. Teknic - ClearPath
    2. Gecko 203V
    3. Gecko G340
    4. Gecko G540
    5. Leadshine MX4660
    6. Leadshine CS-D1008
    7. Longs Motors
    8. CNCdrive - DG4S-16035
    9. DMM - Dynamic Motor Motion
    10. VEXTA
    11. Viper
    12. Mitsubishi - MR-J3
    13. PoStep60
    14. Panasonic
    15. Automation Technology Inc.
    16. Hiwin
  22. Spindle Drives (VFDs)
    1. Bosch Rexroth VFD
    2. Delta C200 VFD
    3. Delta MS300 VFD
    4. Delta VFD-M
    5. Yuhuan Huanyang
    6. Lenze VFD
    7. Hitachi VFD
    8. TECO Westinghouse VFD
    9. Schneider Altivar 18
    10. Mitsubishi FR-D720S-100
  23. Plasma - Torch Height Control
    1. Hypertherm 45XP
    2. Proma Compact THC 150
    3. Torch Touch (floating head) Signal
    4. Torch Breakaway Signal
  24. Mill - Tool Changers
    1. Manual Tool Change
    2. Linear Tool Changer
    3. Umbrella Tool Changer
  25. Lathe - Tool Changers
    1. Manual Tool Change
    2. Linear - Gang Type Setup
    3. 4 Station Turret
    4. 4 Bit Digital Signal Output Turret
    5. Hercus PC200 - 8 Tool Turret
    6. Pragati BTP-63, BTP-80, BTP-100, BTP-125
  26. Upgrading / Unlocking the Controller
  27. OEM Logo & Details
  28. Reporting Bugs and Issues

G28 – Return To Machine Home #


 

CAUTION: This command can be used in different combinations and wrong command can result in unexpected rapid motion. Depending if the machine is in Absolute or Incremental mode the behaviour of G28 command will be very different, extra caution should be used when using this command.

 

 

 

This command is used to move the axis back to the home position of the axis after the machine was homed. Further axis commands can also be combined with G28 to achieve  intermediate position.

 

Syntax & Parameters

  • G28 – Only G28 can be used, this will move all axis at rapid back to the home position.
  • X, Y, Z, A, B Value – specifies the intermediate position you wish to move following the distance to move. The distance value will be the current machine units in use.
  • Combining the G28 with a rotary axis in incremental mode G91 will allow the axis to unwind in 1 revolution or less. See example below.

 

Example program for moving all together axis to home position

N10 G28
The above gcode will move all axis of the machine at rapid back to the home position.

 

Example program all axis to machine 0.00

N10 G91 G28 X0 Y0 Z0
The above gcode will move all axis to machine 0.00 as there is no intermediate position to go to first.

 

Example program to move Z axis first

N10 G91 G28 X0 Y0 Z8
The above gcode will first move the Z axis to 8.00 position and then move all axis to machine 0.00

Rotary Axis Unwind within one rotation

G00 A900   Rapids the A axis to A900 (2.5 turns)
G91         Change to Incremental mode
G28 A0      Moves Axis by 0 degrees then moves to A0 within one rotation
G90         Return to Absolute mode

Notes
  • In the above example if you Specify another coordinate eg: G28 A360 it will move an additional 360 degrees 
    taking the axis to A1260 (3.5 turns) then move to A0 in less than 1 rotation.
    In this case it would be an additional 1/2 rotation to be back to home.
  • If you do not change to incremental mode before the G28 A0 the axis will unwind the full 2.5 revolutions to A0 and
    then move to the home position. In this case no further move is needed.
    
  • This works with both the A and B axis when in rotary mode.
Yes No Suggest edit
Last updated on October 29, 2019
0 of 0 users found this section helpful
Suggest Edit