CNC Services Northwest

Method 3: Use imaginary reference tool for X, normal tool for Z

For CNC11 v3.08 and later, and CNC12

This method is probably the most convenient for most users.



Preparation (one-time)

This procedure will set the X position that is displayed on the DRO while the carriage is at home to a suitable value. If we did not do this, the spindle would want to wind up to maximum speed whenever we went to or from home for a tool change with constant surface speed mode active.

The X Position value you set in step (3) below should be a round number, somewhere close to the maximum swing of your lathe (e.g. 6", 8", 16", 30", etc.).

  1. Press TOOL CHECK to move the carriage to home.
  2. Go to X axis Part Setup (F1/Setup, F1/Part, F8/X axis).
  3. Enter Position=maximum swing, Tool=0, Set All WCS=Yes.
  4. Press F10 to set.

Operation (for each job)

  1. Load all the tools into their tool holders.
  2. Put the first tool in the tool post (or index the turret as needed).
  3. Put a piece of stock of known diameter in the chuck or collet, or turn the job stock to a true-running diameter and then measure it.
  4. Go to Z axis Part Setup (F1/Setup, F1/Part).
  5. Jog the tool in to touch the end of the stock.
  6. Enter Position=0.0, Tool=0 (regardless of the actual tool number).
  7. Press F10/Set to set Z zero here.
  8. Without moving the tool, go to the Offset Library (ESC, F2/Tool Offset).
  9. In the Tool Offset Library, press F2/Measure Tool to get to measuring options.
  10. With any Z Offset highlighted, press F1 to set Z Reference.
  11. Press F10/Set to set Z Reference here.
  12. With the tool still touching the surface, highlight its Z Offset and press F6/Measure Offset Z, then press F10. The resulting offset measurement should be 0.0 (this is the Z reference tool, so it has no Z offset).
  13. Now jog around to touch an outside diameter.
  14. If the stock runs true, just touch the tool to the stock.
    If the stock does not run true, use the jog keys to take light turning cuts until it does run true, then, without moving the X axis from the final cut position, mic the resulting diameter.
  15. With any X Offset highlighted, press F1 to set X Reference Diameter.
  16. Type the stock diameter into the box and press F10.
  17. Highlight the X Offset for this tool and press F5/Measure Offset X, then press F10.
  18. For each remaining tool:
    1. Load the tool.
    2. Highlight the offsets for that tool number.
    3. Jog to touch off on the outside diameter.
    4. Press F5, then F10, to measure the X Offset.
    5. Jog to touch off on the end of the stock.
    6. Press F6, then F10, to measure the Z Offset.
  19. Press F10 to save the measured offsets.

If you have to replace one tool

If the surfaces you used before are still available:

  1. Go to the Offset Library.
  2. Load and measure the new tool off the same surfaces you used before.

If the surface you used before is no longer available (moved or cut away):

  1. Go to the Offset Library.
  2. Load the tool you used as the reference tool before.
  3. Jog it around to touch a new Z face (any Z face).
  4. With a Z offset highlighted, press F1 and set a new Z Reference here.
  5. Load the new tool and measure its Z Offset using that same new face.
  6. Mic any available diameter.
  7. Highlight the X Offset.
  8. Press F1 to set X Reference.
  9. Type in the measured diameter and press F10.
  10. Jog to touch the new tool to that diameter.
  11. Press F5 to measure the X Offset.
  12. Press F10 to save the measured offsets.

To use these same tools on a part of a different length

  1. Go to Part Setup (F1/Setup, F1/Part).
  2. Load any tool.
  3. Jog it in to touch the end of the stock.
  4. Enter Position=0.0.
  5. Enter the correct tool number.
  6. Press F10/Set to set Z zero here.

Copyright © 2016 Marc Leonard
Last updated 14-Apr-2016 MBL