Measuring and Using Tool Length Offsets

Tool Length Offsets (TLO's) are easily measured using the optional DeskCNC Digitizing Probe/Tool Sensor.  There are several methods for machining with TLO's.  Below lists just one method.

TLO's are measured using the M96 or M97 codes.  M96 moves to the Tool Sensor Location defined in menu Setup - Machine Setup - Digitizing Probe.  M97 does not move to location but rather moves directly 'down' to the tool sensor.  M97 is used when the tool sensor is manually moved/placed under the tool for measurement.  M96 is used when the tool sensor is semi-permanently mounted to a fixed location on the machines table.

Measuring TLO's:
1.    If  using M96, set the tool sensor location in menu Setup - Machine Setup - Tool Sensor - X/Y Location along with the Tool Sensor Height. The Sensor Height is relative for this method of calculating TLO's so it does not have to be entered exactly.  Make certain that the Default Lim Polarity is set to Normally Closed when using the Digitizing Probe or Tool Sensor.

2.    Tool Changes are executed using a Tx M6 combination.  A tool needs to be loaded for the M96/M97 commands to function.  Enter T1M6 in the MDI box and press Enter.  The Tool 1 'Tool Change Script' will be executed (Tool Change Scripting).  Tool 1 should now be in the Spindle.

3.    Place the Tool Sensor under the tool and  Enter M97 in the MDI box.  TLO's are measured using the current feedrate.  Enter a new feedrate (F) if warranted.

4.    The Spindle will lower the Tool to the Sensor and record the TLO.  The TLO will be active.  The TLO for Tool 1 will NOT be saved in the Tool Library until you save the Tool Library from menu Setup - Tool Library - Save.  You can measure all tools and then save the entire table.

5.    Once a TLO has been measured, it will need to be active when machining.  This is done with the G43 Hx command where x is the tool number.  The G43 Hx may be placed in the Tool Change Script.

6.    When the Spindle is Zeroed, the Active TLO is used.

Using TLO's when machining:
1.    Place the first tool used in your GCode file in the Spindle.  Do this be entering T1M6 (assumes Tool 1) in the MDI box.  The tool change script for Tool 1 will be executed.  The Tool Change Script should include the G43 H1 command to make the TLO for tool 1 active.  The TLO readout in DeskCNC will display the current TLO.

2.    Zero the tool to the part material.  The Z Coordinate will reflect the active TLO.  

3.    Run the GCode file.  All subsequent tool calls will place the tip of each tool at the proper Z Height according to their TLO.