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.
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
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
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