191

Locate the block number shown in the alarm display and review the part program at that line.

Verify the helical block contains ONLY G02 or G03, arc center parameters (I, J, K or R), the circular plane axes (e.g., X, Y), and ONE additional axis for the helix (e.g., Z).

Remove any canned cycles, rapid positioning commands, coordinate system commands, or cutter compensation calls from the helical interpolation block.

If tool offset or work coordinate changes are needed, program them in a separate block before or after the helical move.

Check the active plane selection before the helical move: G17 (XY plane, Z is helical), G18 (ZX plane, Y is helical), or G19 (YZ plane, X is helical).

Verify the helical axis is NOT one of the two axes defining the circular arc. For example, with G17 active, only Z can be the helical axis, not X or Y.

Ensure the plane selection G-code (G17/G18/G19) is programmed before the helical interpolation block, preferably in the program header or tool change section.

Correct the program by either changing the plane selection or repositioning the helical axis parameter to match the intended toolpath geometry.

Calculate the arc radius using the I, J, K incremental values from the start point, or verify the R value if radius programming is used.

Radius programming (R) can be ambiguous for arcs greater than 180 degrees; use I, J, K for helical moves when possible.

Verify the start and end points in the circular plane (e.g., X and Y for G17) are not identical. If they are, this creates a full circle helix which may require parameter setting or different programming method.

Check that the distance from start point to arc center equals the distance from end point to arc center (equal radii). A mismatch exceeding the control's tolerance triggers programming errors.

Recalculate and correct the I, J, K values or endpoint coordinates to ensure valid arc geometry, then re-verify with graphic simulation if available.