Why Does Fadal VMC15 Overtravel During Tool Changes?

The Z axis exceeds its travel limit during a tool change because Z0 H0 cancels tool length compensation while the fixture Z offset remains active. Adding E0 removes that Z-offset contribution, but it also changes the active X/Y coordinate frame, so subsequent X/Y targets can shift or overtravel. On the VMC15 with 88HS control running Format 2, use the tool-change function to coordinate those cancellations, then handle the end-of-program position with a verified machine-coordinate or dedicated fixture-offset move.

Position Past the Travel Limit

The number that matters is the commanded machine position after every active offset has been applied. An overtravel occurs when that result lies outside the axis travel envelope; the programmed value can still look harmless. A commanded Z0 is not necessarily machine Z zero when a fixture Z offset or tool length offset remains active.

Read both the work-coordinate and machine-coordinate displays while single-blocking. The work display describes the selected programming frame; the machine display decides whether an axis can physically reach the target.

Offset Arithmetic Behind the Symptom

Tool length compensation and fixture Z compensation solve different geometry. A preset tool length describes the distance associated with a tool relative to a stable spindle-based reference. The fixture Z value describes where the part origin lies relative to the machine or table reference. The control combines those values with programmed Z to obtain an axis target.

When tools are touched directly to part zero and fixture Z is zero, canceling the H value near Z0 may appear to work because there is no significant fixture-Z term left in the calculation. Moving tool measurement to the table changes that arithmetic: the tool values become reusable, while the fixture carries the part-origin height. A postprocessor sequence that was harmless under the first convention can then command a target outside Z travel.

For the reported 88HS Format 2 workflow, M6 cancels the tool length offset and the Z component of the current fixture offset together as part of the tool change. That coordinated transition is why a minimal sequence such as M5 followed by T2 M6 avoids the intermediate state created by Z0 H0. The risk is clearance: a tall part, fixture, or long tool can intersect the setup while the head moves to the tool-change position.

Selecting E0 before the tool change addresses more than Z. The E register represents a coordinate frame containing X, Y, and Z components. Changing it can therefore alter the coordinate interpretation of all three axes. If the postprocessor issues or retains X/Y targets around that transition, visible lateral motion is a coordinate-state effect, not random servo drift.

Tool-Change Procedure

Remove the premature offset cancellation from the post and prove the machine’s native tool-change behavior at reduced operating risk. Use this sequence as the starting pattern shown for the installation:

M5
T2 M6

1. Record the active fixture number and its X, Y, and Z values. Record the current tool number and H value before editing the post.
2. Delete Z0 H0 and the added E0 from the line immediately before the tool change. Those commands create separate coordinate-state transitions that the tool-change function already handles in this workflow.
3. Stop the spindle with M5. On this control workflow, that command was also used to cancel M7 and M8.
4. Call the next tool with Tn M6, substituting the required tool number for n.
5. Run the sequence in single block with rapid override reduced. Watch machine Z, the distance-to-go display, and the physical clearance above the tallest setup feature.
6. After the change, confirm that the program reselects the required fixture and tool compensation before the next cutting move. Read the actual E and H states on the control instead of inferring them from the CAM operation name.

Clearance must be decided before committing to automatic operation. If the tool-change trajectory crosses a tall workpiece, move to a known safe machine-coordinate Z position first, using a syntax already verified for this control and post format. Offset cancellation alone does not create physical clearance.

End-of-Program Positioning

In the sequence below, the second line sends the table toward the home position; it does not command a corresponding spindle retraction:

Z0 H0 M05
X0 Y0 E0 M02

The first line can overtravel Z because fixture Z remains active after H0. The second line combines X/Y positioning with selection of E0, making the final target dependent on the control’s execution of that block and the values associated with the departing and selected coordinate frames.

Two demonstrated alternatives separate the final positioning intent more clearly. One uses machine coordinates:

G53 Z0
X0 Y0 Z0 E0 H0
M6 T1
M30

This pattern retracts Z with G53 Z0, then positions X, Y, and Z with offsets cleared, calls tool 1, and ends with M30. Verify how the 88HS control applies G53 to each block before adopting the sequence; machine-coordinate commands normally apply only to the block in which they are programmed.

The other alternative uses a dedicated fixture entry:

G0 X0 Y0 Z0 E47 H0

In the documented setup, E47 usually contained X0, Y8, and Z0. When a fixture was displaced in X, its E47 X value was changed, for example to X-10. The next register, E48, was reserved there for an electronic tool-length touch probe. Those register assignments are installation-specific; inspect the offset table before using either identifier.

Reusable Tool-Length Workflow

Measuring every tool from a stable spindle-based reference separates tool geometry from job geometry. The tool length remains associated with the tool, while each setup requires X, Y, and Z fixture pickup. This supports multiple operations on one table and allows a common tool to serve several operations without retouching it to every part zero.

An offline tool setter can supply those reusable tool-length values. A height gauge and indicator can provide the same reference strategy when the presetter is unavailable, provided the measurement datum matches the machine’s established tool-length convention. A control-mounted probe can also measure tools, but its cycle time may make repeated setup changes less attractive.

Presetting reduces repetitive tool touch-off, but it transfers more responsibility to fixture-offset control. Confirm the sign, datum, and units of the fixture Z entry every time the setup changes. A reusable tool number is safe only when the physical tool, holder, stored length, and programmed H call still match.

Controlled Verification

1. Back up or record the current E and H tables and retain the original post output for comparison.
2. Place the machine where every axis has room to move. Remove the workpiece or use a clearance condition that prevents contact during the first test.
3. Load a short test containing spindle stop, one tool change, offset reselection, a noncutting approach, and the intended end sequence.
4. Single-block through the line before M6. Confirm that the post has not emitted Z0 H0 or an unintended E0.
5. At the tool change, compare machine Z before and after the control cancels compensation. Stop if distance-to-go points beyond the usable stroke or if clearance decreases toward the setup.
6. After the new fixture and H values are active, command a point well above the part and verify its measured relationship to part zero.
7. Single-block the end sequence. Confirm the selected E register, then check that the requested X/Y endpoint lies inside travel before allowing full rapid.
8. Repeat with the tallest fixture and longest intended tool because those produce the smallest physical clearance even when the coordinate arithmetic is correct.

A successful test has three independent results: no axis limit request, correct physical clearance during the tool change, and correct tool-tip position after the work and tool offsets are restored. Passing only the first result does not validate the setup.

Recurring Offset Pitfalls

Postprocessors often inherit assumptions from the tool-setting method used when they were created. Changing from job-specific tool touch-offs to table-referenced lengths changes where Z geometry resides, so every automatic H0, E0, return-to-zero block, and first approach move requires review.

A combined block also hides sequencing questions. Separate coordinate-system selection, compensation selection, and axis motion during commissioning so the displayed state can be checked after each action. Once verified, combine commands only where the 88HS Format 2 execution behavior is known.

Memory-based tool corrections are another recurring failure mode. A value remembered from the previous setup can be paired with the wrong holder or fixture datum. Maintain the tool-length record with the physical tool identity and verify it after insert, holder, gauge-line, or measurement-reference changes.

Finally, an axis home-end position is not automatically a safe setup position. A dedicated E register such as E47 can encode a convenient unload location, but its stored values must match the current fixture arrangement. Label reserved registers and check them before a post-generated move uses them.

Frequently Asked Questions