Configuring Syntec 6MD Automatic Tool Length Offsets

After the fix, every measured holder can reference the same table surface, while G54 Z accounts for stock thickness when the program zero is on top of the workpiece. The working chain is: fixed tool setter → tool-length value in offset Hn → G43 Hn → calibrated Delta Z reference → G54 work offset. Changing tools does not require rewriting G54 when that chain is configured correctly.

Where does the tool-length data travel?

Follow the data path. A tool enters the spindle, the Z axis moves it to the stationary measuring sensor, and the controller records a length value in the corresponding tool-offset entry. Selecting that tool changes the physical holder in the spindle; it does not necessarily activate the matching length compensation. The program must apply G43 Hn, where n identifies the offset assigned to that tool.

Stage	Function	Failure symptom
Stationary sensor	Provides the repeatable contact position used during tool measurement	Measurements drift, stop early, overtravel, or target the wrong XY position
Tool table	Stores the measured value for each offset number	Different holders receive missing, duplicated, or implausible values
G43 Hn	Applies offset number n to the active Z coordinate calculation	The correct tool is loaded but its displayed or commanded tip position is wrong
Delta Z or external shift	Relates the tool-measurement system to a chosen physical reference surface	All tools share a similar Z error relative to the table
G54 Z	Relates the reference surface to the program's workpiece Z zero	Tool-to-tool agreement is good, but the entire job is vertically displaced

G41 and G42 compensate the cutter path laterally. They do not solve tool-length differences. The required axial compensation is G43 with the correct H entry.

Which Z-reference method fits the machine?

Two methods worked within the described control arrangement. The external-shift method establishes production coordinates quickly. Calibrating the tool setter against a physical surface creates the cleaner permanent relationship for repeated automatic tool changes.

Method	Reference action	G54 Z use	When to use it	Maintenance consequence
External-shift correction	Touch a calibrated tool to the table and enter the displayed table error in the external Z shift; one setup used 8.137	Enter the stock-thickness relationship when program Z zero is on the stock top	Fast recovery when the tool offsets work but table Z does not display zero	Keep the shift under configuration control; an unexplained change moves every job
Tool-setter datum calibration	Touch a calibrated tool to the chosen surface, open Offset → Tool Tip Measure, and press F3	Normally represents stock thickness above the table for top-referenced programs	Recommended permanent setup for a fixed sensor and interchangeable holders	Remeasure all tools after changing the datum because Delta Z changes

Use the second method for normal operation. It makes the table, fixture surface, or another deliberately chosen plane the common tool-tip datum. Use the first method as a controlled correction or diagnostic, not as a substitute for finding unstable measurement hardware.

If every part has the same thickness, the stock top can itself become the calibrated reference. In that special case, Z work offsets may remain at zero. A table-based reference is more flexible when stock thickness changes: measure tools once against the table, then change only the work-offset relationship for each job.

What must be checked before changing offsets?

Layer one first. Inspect the stationary sensor, its mounting, the approach point, and the complete magazine-to-spindle motion before editing coordinate values. A numeric correction cannot repair a moving sensor, a loose holder, an incorrect pocket position, or a calibration move aimed at the wrong XY location.

1. Confirm that the tool setter is stationary and firmly mounted. Verify that its contact surface returns freely and that chips cannot hold it down.
2. Check that the holder seats consistently in the spindle and that each magazine pocket releases it without forcing the retaining hardware.
3. Confirm the active tool number, the intended offset number, and the value written into that offset after measurement.
4. Review the sensor target coordinates before starting calibration. If lost coordinates make the cycle travel toward X0 Y0, stop the cycle and recover the configured target from the machine configuration, calibration macro, or a known-good backup. The evidence supplies no universal Syntec parameter number for these coordinates.
5. Use single-step control, a low motion override, and MPGSIM handwheel authorization where configured. Keep a hand on feed hold during the first approach.

One test forced the Z axis hard enough to bend the magazine retaining beam. Treat drifting coordinates or unexpected downward motion as a stop condition. Retract in a controlled direction, remove the at-risk holder if the machine procedure permits it, and correct the target or offset state before continuing.

How should the table reference and tool offsets be calibrated?

1. Back up or record the current tool offsets, G54 Z, external Z shift, and displayed Delta Z. These values reveal whether the later change affected individual tools or the common datum.
2. Set unintended Z values in the work offsets and external shift to zero for the diagnostic baseline. Do not erase unrelated axes.
3. Load a known tool and run the machine's tool-measurement cycle against the fixed sensor. Verify that its value appears in the intended tool-table entry.
4. Activate the same tool and offset explicitly, for example G54 T1 G43 H1. Loading T1 alone does not establish that H1 is active.
5. Move the calibrated tool tip carefully to the selected reference surface. For the usual table-based arrangement, touch the table surface using the machine's accepted manual touch-off method.
6. Open Offset → Tool Tip Measure and press F3. This establishes the common tool-tip reference and changes the associated Delta Z relationship.
7. Remeasure every tool. Values measured before the datum change belong to the previous reference relationship.
8. For a program whose Z zero is at the top of the stock, set G54 Z from the measured stock thickness and the controller's displayed coordinate convention. Jog to the stock top and verify that the active work-coordinate Z reads zero before running code.

The critical pairing is one-to-one: T1 G43 H1, T2 G43 H2, and T3 G43 H3. A command such as T2 G43 H1 loads tool 2 while applying tool 1's length value. The resulting Z discrepancy can be approximately the physical difference between those holders.

How should production programs handle automatic changes?

Each tool-change block must select the new tool and activate its matching length offset before any Z move that depends on the tool tip. In this installation, selecting T2 did not automatically activate H2; the required state was T2 G43 H2. Apply the same rule to every pocket unless the machine builder's tool-change macro explicitly performs and verifies that action.

G54
T1 G43 H1
...
T2 G43 H2
...
T3 G43 H3

Do not measure every holder again after every normal tool change. Measure a holder when it is installed, replaced, reseated after a suspected collision, or when its recorded length is no longer trustworthy. With a stable sensor and a valid table reference, the controller reuses the stored Hn value.

Do not edit G54 Z for each holder. G54 describes the workpiece coordinate system; Hn describes the individual tool. Rewriting the work offset to hide a tool error makes the next correctly measured tool wrong.

How do the symptoms identify the failed stage?

Observed result	Likely failed stage	Decisive check	Correction
Tool 1 reads zero at the surface, but tool 2 reads a large Z error	Wrong or inactive H offset	Confirm the block contains T2 G43 H2, not T2 or T2 G43 H1	Activate the offset matching the loaded tool
Every tool stops at a different physical height after calibration	Tool-table values, sensor repeatability, or tool-to-offset mapping	Compare table entries and repeat measurements without changing the holder	Repair the measurement path, then remeasure all tools
Every tool has nearly the same error from the table	Common Delta Z, external shift, or work-offset error	Touch one calibrated tool to the reference surface and read the common Z error	Recalibrate with Tool Tip Measure → F3 or apply the controlled external correction
G43 H2 appears to do nothing at machine zero	Wrong coordinate display selected	Compare the displayed absolute coordinate before and after executing G43 H2	Use the display that reflects active compensation; no axis motion is required
Calibration travels toward X0 Y0	Lost tool-setter target coordinates	Inspect the calibration target in the machine configuration or macro	Restore the commissioned coordinates before moving toward the sensor
The same holder produces different offsets in different pockets	Pocket mapping, holder seating, or measurement repeatability	Measure one unchanged holder from multiple pockets	Correct the pocket or measurement path producing the different value

Executing G43 H2 at machine zero should complete quickly and need not move an axis. Its visible effect is a coordinate transformation: the applicable absolute display changes by the value of the second tool offset. A brief busy indication followed by no physical movement is normal. If the correct display changes by the correct offset, G43 is active.

How is the complete setup verified without cutting?

First compare one unchanged holder across magazine pockets. Measure it from two or more pockets without altering its gauge length. The corresponding measured values should match within the machine's repeatability. A material difference isolates the fault to pocket mapping, seating, or the measurement sequence rather than cutter length.

Next confirm compensation numerically. Move to machine Z zero, execute each G43 Hn, and record the before-and-after absolute Z display. The change must correspond to the selected Hn entry. Repeat for H1, H2, and H3.

Only after those checks, use the documented clearance test. The original test sequence was:

Tn G43 Hn
G0 X100.0 Y100.0 Z50.0
G1 Z20.0 F500.0
G0 Z50.0

This sequence assumes millimetres, a valid table-based datum, and a clear position at X100.0 Y100.0. Confirm those conditions before executing it. Run each holder separately with MPGSIM, single-step control, and reduced motion override. Each correctly measured tool should stop with its tip at the same commanded height, 20.0 mm above the table. Finally activate the production G54, jog each tool to the stock top, and verify that work-coordinate Z reads zero without changing G54 between tools.

FAQ