506

Check Parameter 85 Current Value

Press SETTING, scroll to PARAMETERS, enter 85, verify current tolerance value (default 0.0002").

Examine Failing G02/G03 Block

In EDIT mode, locate the exact line causing alarm. Calculate start radius √((X-start - I)² + (Y-start - J)²) and end radius √((X-end - I)² + (Y-end - J)²).

Verify CAM Post-Processor Settings

Check CAM post-processor decimal precision settings. Increase coordinate and IJK output to minimum 4 decimal places for inch programs.

Many Haas users set Parameter 85 to 0.0005" to accommodate typical CAM rounding while maintaining arc quality.

Regenerate G-Code with Higher Precision

Re-post the toolpath with increased decimal precision or smaller arc tolerance in CAM system.

Identify Problem Arc Block

Note the N-block number from alarm display, press RESET, then EDIT to locate the failing G02 or G03 command.

Verify Arc Center Calculations

For G02/G03 with I, J values: ensure I = (arc_center_X - start_X) and J = (arc_center_Y - start_Y). Use calculator to verify math.

Use R-format (G02 X__ Y__ R__) instead of IJK format for simple arcs to let the control calculate the center.

Check Arc Quadrant Logic

Verify arc doesn't exceed 180° when using IJK format. For arcs >180°, break into multiple smaller arcs or use R-format with negative radius.

Test with Graphics Verification

Press GRAPHICS, run program in single block mode to visually verify arc geometry before cutting.

Check Active Work Offset

Press OFFSET, verify which work coordinate system (G54-G59) is active and confirm offset values are correct.

Verify G52 Local Coordinate Usage

Search program for G52 commands that may shift local coordinate system. Ensure G52 X0 Y0 Z0 is used to cancel before arc moves if needed.

Test in Machine Coordinates

Temporarily modify program to use G53 (machine coordinates) for the problematic arc to isolate coordinate system effects.

G53 moves are in machine coordinates - ensure adequate clearance from fixtures and table edges.

Recalculate Arc in Correct Coordinate System

Adjust I, J, K values or endpoints to account for active work offset coordinate system.

Compare with Original Program File

Check original CAM output or proven program file against current program in Haas memory using EDIT mode line-by-line comparison.

Verify DNC Transfer Integrity

If using RS-232 or Ethernet transfer, re-send program file. Check Parameter 20 (RS-232) settings: 9600 baud, 8 data bits, 1 stop bit, no parity.

Check for Incomplete Line Transfers

Look for truncated lines or missing characters in G02/G03 blocks. Common issue is missing decimal points or dropped digits.

Use Haas DNC software or verify checksums when available to ensure complete file transfer.

Reload Clean Program Copy

Delete corrupted program (EDIT, then DELETE PROGRAM) and reload from verified source file.

Review Parameter 85 History

Press SETTING, PARAMETERS, enter 85. Check if value was modified from default 0.0002". Note current setting.

Test with Relaxed Tolerance

Temporarily increase Parameter 85 to 0.0005" and re-run program to verify arc geometry is actually valid.

Only qualified personnel should modify machine parameters. Document original value before changes.

Evaluate Arc Quality Requirements

Consider part tolerance requirements vs. Parameter 85 setting. Most applications work well with 0.0002" to 0.0005" arc tolerance.