Service Home 5-Axis Troubleshooting - CHC - TG0015
Last updated: 01/27/2026

5-Axis Troubleshooting Guide -CHC

TG0015

Programming

Symptom

 Solution
The program does not load. Make sure there is a percentage sign (%) at the top and bottom of the program.
Make sure the program number starts with the letter "O" and is followed by 5 numerical digits.
Make sure that text in parentheses is shorter than 80 characters, including spaces.
Check for G-Code errors on the Alarms Messages screen.
Refer to the sample program, below.
The program loads, but everything is in parentheses. Make sure that the inch or metric value in Setting 9, Dimensioning, matches the program.
If the program is a macro, make sure that Parameter 57:22, Enable Macro, is set to 1.

                       Sample Program

% (The % sign is needed only when you load a program from an external device)

O00001 (The program number must start with letter O followed by a 5-digit number) ;

G00 G17 G40 G80 G90 G54 (CAM systems usually post out this safety line) ;

T1 M6 ;

G54 G90 G00 X1.25 Y1.3 S3000 M03 ;

G43 Z1. H01 Z.1 M08 ;

(PROGRAM CONTENT HERE) ;

G90 G53 Z0. ;

G90 G53 Y0. ;

M30 ;

% (The % sign is only needed when loading a program from an external device)

Motion

Symptom Solution
The program jolts or the control hesitates when the program runs. Set the IN POSITION LIMIT parameters to 16000 for sigma 1 rotary products, or to 128000 for Sigma 5 rotary products:
A-Axis: Parameter 104
B-Axis: Parameter 165
C-Axis: Parameter 512
Make sure that the program does not have more than 1000 blocks per second.
Make sure the 4- or 5-axis program uses G93 for synchronous moves. Make sure that the maximum feedrate is F45000.
Run the Parameter Checker Program (menu option 7) to compare the parameters to the factory-installed parameters.
For G02/G03 moves, make sure the I, J, and K values are posted to 4 decimal places for inch mode, or 3 decimal places for metric mode.
A canned cycle moves in the wrong direction. Before it calls a canned cycle, the program must give the the plane and the spindle direction. In 18 series software, the control does canned cycles in all 3 planes (G17, G18, and G19), and to respect the spindle commands M03, M04, and M05.
The part shows witness marks. Make sure the CAM system posts M11 and M13 to release the brakes on the rotaries before making a 5-axis simultaneous cut.
Radiused curves are faceted. There are not enough lines of code if a G01 (or point-to-point) code is used when machining a radius. Adjust the cut tolerance and stroke length settings in the CAM program.

Settings 34 and 79

Make sure that Setting 34, 4th Axis Diameter, and Setting 79, 5th Axis Diameter, are both set to the correct diameter. The default value in these settings is 1.

If the diameters are not correctly set, you could get unusual results.

For example, if Setting 34 and Setting 79 are set to 1 when the part has a 3 inch diameter, the actual feedrate around the circumference of the part is (3) times faster than the programmed feedrate. This can cause problems with the surface finish. Or, this can cause broken tools.

For example, if Setting 34 and Setting 79 are set to 3 when the part has a 1 inch diameter, the time to machine the part is (3) times longer than usual.

It is also possible that the programmed feedrate is higher than the rotary's capability.

Make sure the rotary feedrate is not higher than the maximum degrees-per-minute (DPM) specification. Refer to the advertised specification. Calculate the DPM from the programmed feedrate and diameter.

VR Machines

The VR series mills have a unique 5-axis capability. This requires special care in programming:

  • Make sure the tool length is set up correctly.
    • G143, Tool Length Compensation is unique to the VR series.
    • G143 compensates for the tool length along the axis vector when the A and B Axes are tilted.
  • Calibrate the tool probe to the gage line of the machine.
    • For most 3-axis machines, you calibrate the tool probe to the face of the spindle. Do not do this for the VR.

UMC-750

Machine Rotary Zero Point (MRZP) Offsets

  • MRZP Offsets are control parameters which define the centers of rotation for the rotary table. The centers of rotation are the home positions of the linear axes. See the UMC-750 Operator's Manual for the correct procedure to set these.
  • The MRZP parameters are used whenever G234, Tool Center Point Control (TCPC), and G254, Dynamic Work Offsets (DWO), are active in a program. If the MRZP parameters are not set correctly, the machine does not go to the correct position when G234 and G254 are active.