Troubleshooting Mazak Nexus 350 G71 Radius Compensation

898 LAP CYCLE ILLEGAL SHAPE DESIGN appears because the Mazatrol Matrix control cannot construct a legal G71 roughing path from the contour between P10 and Q20 when G42 is activated on N10. The earlier Fanuc program depends on control-specific behavior that ignores compensation during roughing and applies it during G70 finishing; that behavior is not portable to Matrix. First prove the uncompensated contour with G40, then implement tool-nose compensation using a lead-in and cycle arrangement explicitly supported by the machine's EIA programming manual.

Symptom and decision path

The number that matters is the stored tool-nose radius. G42 moves the calculated tool-center path away from the programmed part contour by that radius. At every corner, the control must find a valid intersection or tangent between adjacent offset segments. If it cannot create that geometry while expanding the G71 LAP contour, it rejects the cycle before cutting.

In the submitted program, compensation starts on the first referenced contour block:

N10 G00 G42 X0
G01 Z0
X20
Z-10
X35
Z-30
X40
N20 G40

The machine approaches from X40 Z1, activates G42 during a rapid X move to X0, changes direction at the following block, and cancels compensation at N20. That combines compensation engagement, the first LAP-cycle profile block, rapid motion, and a corner. Separating those functions is the first corrective action.

Observed result	Likely cause	Next check
898 disappears after removing G42 and G40 from N10-N20	Compensated geometry or compensation placement is illegal for the cycle	Check the Matrix EIA manual's G71/G70 compensation rules and add a separate lead-in
898 remains with G40	The LAP profile shape or block format is invalid independently of compensation	Validate the first profile block, contour direction, endpoints, and every transition
The cycle runs, but the finish size is displaced	Compensation is absent, duplicated, or using incorrect tool data	Verify nose radius, tool orientation, active offset system, and compensation side
The tool-eye values exist, but EIA motion is still wrong	The program is calling an EIA offset register rather than the Mazatrol tool-data coordinate system, or vice versa	Check the active coordinate method and decode the complete T word

Tool-nose compensation geometry

G41 and G42 select opposite sides of the programmed path. The correct side follows from tool travel direction, whether the cut is on an outside or inside surface, and the control's tool-orientation definition. It cannot be selected from the tool number alone. An incorrect side can offset the tool into the material or create an impossible corner.

Compensation needs motion over which the control can establish the offset path. A useful lead-in is geometrically distinct from the finished contour and long enough relative to the stored nose radius and the direction change. A zero-length engagement, engagement directly at a finished corner, or immediate reversal can leave no valid intersection. Starting compensation on a rapid block inside a LAP definition also makes the roughing-cycle interpreter responsible for geometry that an ordinary finishing path might accept.

This is geometry, not logic. The control can have valid tool data and still reject the path because the compensated segments do not meet. Conversely, deleting G42 can clear the alarm while producing the wrong finished contour if the coordinates describe the nominal part rather than the tool-center path.

Matrix and Fanuc cycle differences

The control is Mazatrol Matrix. Its EIA G-code type is fixed to the modern lathe format described by its programming manual; it does not offer the older selectable Type A, B, or C compatibility behavior associated with Fusion controls. A Fanuc-format G70-through-G76 cycle therefore requires a block-by-block review before use on Matrix.

The original program assumes that G42 inside the P10-to-Q20 definition is ignored by G71 but becomes effective when G70 P10 Q20 reuses the same blocks. Matrix instead validates the referenced contour under its own LAP-cycle rules. Copying the syntax preserves the text, not the source control's interpretation.

Use the Matrix EIA programming manual to answer three machine-specific questions: whether compensation may be active while G71 reads the profile, whether G70 inherits or reevaluates compensation in the referenced blocks, and which addresses are permitted in the first P block. Those answers determine whether one shared contour can support both cycles or whether the finish pass needs a separately programmed path.

Tool data, offsets, and coordinates

Touching a tool on the tool eye and defining it as an outside, inside, or grooving tool populates Mazatrol Tool Data. That does not by itself prove which values an EIA program is using. Matrix can distinguish Mazatrol coordinate/tool data from EIA offset registers, and the selected coordinate method must match the T-word convention.

With a four-digit tool call, the documented format in the supplied setup information is TAABB: AA selects the turret station, and BB selects the EIA offset register when that register is intended. The machine can also be configured for a six-digit T word. Read the T-word section of the machine's EIA manual and the active machine configuration before translating an existing T0101 or T0202 call.

Item	Quantity or selection	Where to read it
Tool-nose radius	Radius used to offset the programmed contour	Active Mazatrol Tool Data entry or EIA offset register
Tool orientation	Inside/outside use and nose-direction definition	Tool Data or active geometry-offset display
Turret station	AA in a four-digit TAABB call	Programmed T word and turret display
EIA offset register	BB when four-digit EIA offset selection is used	Programmed T word and offset page
Coordinate method	Mazatrol tool-data coordinates or EIA offsets	Program header, active modal display, setup page, and EIA manual
Part Z reference	Program-specific Z offset	Setup page associated with the active program

The Mazatrol coordinate method may be selected with G53.5 or G53, depending on the installed configuration. Under that method, the program's setup-page Z offset and the indexed tool's Tool Data remain associated with the program and turret station. Confirm the actual selection on the active modal display rather than adding either code from memory.

Controlled correction procedure

1. Record the active program, setup-page Z offset, Tool Data entry, EIA offset entry, full T word, and modal G-code display. This establishes which coordinate and compensation data the control is using.

2. Confirm that the program is running as Matrix EIA/ISO code. Review the Matrix format for G71 and G70; the source control's cycle syntax is not the acceptance test.

3. Check the literal program text. If GOO appears on N10 rather than the digit-based G00, correct that transcription error before evaluating the contour.

4. Force G40 before the roughing cycle and temporarily remove G42 and the matching G40 from the P10-to-Q20 profile. Run the control's graphics or path-check function. If 898 clears, the profile is acceptable without compensation and the diagnostic has isolated compensation placement or compensated geometry.

5. If the alarm remains, simplify the profile without changing its intended endpoints. Test from N10 forward and add one segment at a time until the rejection returns. Inspect the first-block requirements, contour direction, non-tangent corners, reversals, and coincident points.

6. Select one compensation strategy. Either program nominal part geometry and let the control apply the verified nose radius and orientation, or program the calculated tool-center path with G40. Applying both methods duplicates the radius correction.

7. For control compensation, engage G41 or G42 on a dedicated finishing lead-in outside the finished contour and cancel it on a lead-out after the last finished point. If the Matrix manual prohibits that arrangement with a shared G70 profile, program a separate finishing path rather than relying on Fanuc's ignore-then-apply behavior.

8. Verify the T-word interpretation. Confirm that T0101 selects turret station and offset data intended for tool 1, and repeat the check for T0202. If the installation uses six-digit calls or Mazatrol coordinates, translate the calls according to the configured format.

A safe structural pattern is:

G40
G00 [roughing approach]
G71 [Matrix-supported first block]
G71 P10 Q20 [Matrix-supported second block]
N10 [uncompensated LAP profile start]
...
N20 [LAP profile end]

G00 [safe finishing lead-in start]
G41 or G42
G01 [lead-in motion]
[finishing contour or supported G70 arrangement]
G40
G00 [lead-out/retract]

The brackets mark engineering decisions, not executable syntax. Populate them from the Matrix EIA manual, the actual tool orientation, and a collision-checked setup.

Verification and prove-out

Run graphics first and confirm that the roughing passes stay on the stock side of every programmed segment. Then inspect the displayed path at the compensation engagement and cancellation points; neither should create a jump, loop, reversal, or move toward the chuck or fixtures.

Use single-block operation, reduced rapid override, and the site's approved dry-run or machine-lock process for the first physical test. Begin from a verified clearance position and confirm the active tool, spindle direction, work offset, tool offset, and compensation state before cycle start. The program uses G96 constant surface speed with a G50 S3000 limit, so verify that the displayed spindle command remains appropriate for the workholding and part diameter throughout the approach.

After a controlled finish pass, measure a straight diameter and a feature containing a taper or corner. A uniform diameter error points first to X geometry or wear data. Correct straight diameters combined with an incorrect taper or blend points toward nose radius, tool orientation, compensation side, or contour geometry. Recheck the modal display after N20 and after retraction to confirm that G40 has cancelled compensation.

Recurring failure modes

• Assuming cycle compatibility: Identical G-code numbers do not guarantee identical roughing-cycle grammar or compensation handling.

• Compensation inside the LAP boundary: Activating G42 on N10 combines contour definition with offset engagement and can produce 898.

• No independent lead-in: Starting compensation at a finished corner gives the solver insufficient geometry to establish the tool-center path.

• Mixed offset systems: Tool-eye data in Mazatrol Tool Data and an EIA register selected by BB are different sources. An EIA program must intentionally select the intended one.

• Incorrect nose orientation: A valid radius with the wrong directional definition moves the compensated path to the wrong side.

• Compensation applied twice: A pre-offset tool-center program combined with G41 or G42 shifts the path by another nose radius.

• Transcription errors: The shown GOO contains letters rather than zeros if entered literally.

• Safety-system changes used as a programming workaround: Do not bypass the safety shield or machine interlocks to diagnose 898. The alarm is resolved through cycle syntax, contour geometry, and offset configuration.

Frequently asked questions