PS0020

Identify the offending G02/G03 block

Review the program on the CNC control screen to locate the G02 or G03 command that triggered the PS0020 alarm. Note the I, J, and K values specified for the arc center.

Use the alarm message or program cursor to pinpoint the exact line; some controls highlight the problematic block.

Ensure the machine is in a safe, stopped state before editing any program.

Calculate start and end radii

Using the start point coordinates and the I/J/K offsets, calculate the distance (radius) from the start point to the arc center. Repeat for the end point coordinates. Compare the two radii to confirm a mismatch.

Use a calculator or CAD software to double-check manual calculations for accuracy.

N/A

Correct I/J/K values

If a mismatch is confirmed, revise the I, J, or K values to ensure the start and end radii are equal within the tolerance set in parameter 3410. Reload and test the program with a dry run.

Consider switching to R-word programming if repeated errors occur, as it directly specifies radius and avoids this issue.

Double-check edits to avoid introducing new errors in adjacent blocks.

Review CAM output precision

Check the post processor settings in your CAM software for the number of decimal places used in outputting I, J, and K values. Look for settings like 'coordinate precision' or 'output resolution'.

Most modern CAM systems allow precision up to 6 decimal places; set it higher if possible.

N/A

Compare with original toolpath

Export the toolpath from CAM with higher precision settings and compare the I/J/K values in the NC code to the original design coordinates. Look for discrepancies caused by rounding.

Use a text comparison tool to quickly spot differences between old and new outputs.

N/A

Regenerate and test program

Adjust the post processor to output higher precision (e.g., 5 or 6 decimal places), regenerate the NC code, and reload it into the CNC control. Run a dry test to confirm the alarm no longer triggers.

Save the updated post processor settings as default to prevent future issues.

Ensure the machine is in a safe mode during testing to avoid unintended motion.

Check program unit mode

Review the NC program for G20 (inch) or G21 (metric) commands at the start of the code to determine the intended unit system.

If neither G20 nor G21 is present, the program may rely on the machine’s default setting—check documentation.

N/A

Verify machine unit mode

Access the CNC control settings or display to confirm the current unit mode of the machine. Compare it to the program’s intended mode.

Some controls display the active unit mode on the position screen or in system parameters.

N/A

Correct unit mismatch

If a mismatch is found, either update the program to include the correct G20 or G21 command at the start, or change the machine’s default unit setting if permissible. Test with a dry run after correction.

Always include explicit G20/G21 in programs to avoid ambiguity with machine defaults.

Ensure no other programs are affected if changing machine defaults.

Analyze arc angle

Review the G02/G03 block to estimate the arc angle based on start and end points relative to the center (I/J/K). Determine if it exceeds 180 degrees.

Use a CAD drawing or plot the points manually to visualize the arc span.

N/A

Split large arc into segments

If the arc exceeds 180 degrees, edit the program to break it into two or more smaller arcs (each less than 180 degrees) by introducing intermediate points along the arc.

Calculate intermediate points using trigonometric functions or CAD software for accuracy.

Ensure toolpath continuity when splitting arcs to avoid jumps or gouges.

Test revised program

Reload the modified program into the CNC control and perform a dry run to verify that the alarm no longer triggers and the toolpath is correct.

Use graphic simulation on the control if available to confirm smooth arc transitions.

Monitor closely during testing to prevent collisions from programming errors.

Access parameter 3410

Enter the parameter mode on the Fanuc control (often requires a password or specific key sequence) and locate parameter 3410, which defines the arc radius tolerance.

Refer to the Fanuc operator’s manual for the exact procedure to access parameters on your control model.

Incorrect parameter changes can affect machine behavior; proceed with caution.

Check current tolerance value

Note the current value of parameter 3410 (default is often 0.002mm or 0.0001 inch). Compare it to the precision of your programmed coordinates to see if it’s overly restrictive.

If your program uses 3 decimal places, a tolerance tighter than 0.001 may cause issues.

Document the original value before making changes for easy rollback if needed.

Adjust tolerance and test

Increase the tolerance slightly (e.g., from 0.002mm to 0.005mm) to accommodate minor mismatches. Save the change, reload the program, and test with a dry run to confirm resolution.

Make small incremental changes to avoid compromising arc accuracy.

Excessive tolerance increases may mask real programming errors; adjust conservatively.