Program Stops With Spindle Running (G3 CNC)

The most common cause of this condition is loss of encoder signal, especially if it occurs right after a tool call. Verify that the progam is stopped at a g95 block, usually right after a tool call, or at any other block where slide movement depends on spindle speed, such as g33, g83, g96. If this is the case, then the issue is probably encoder‑related.

Tools are generally called to position using g00 (Rapid), or g94f300. These moves are in inches per minute (IPM). When the tool is in position, the mode is usually changed to inches per revolution (IPR), with a g95 block.

The g95 requires spindle encoder pulses for the slide to move, so if the encoder is bad or disconnected, the slide will not move; it is "waiting" for the spindle encoder to "tell it" how fast to move.

NOTE: If your OmniTurn has belt‑driven encoder (GT series:Belt‑driven encoder on GT pre‑2006; Attachments:Belt‑driven encoder on Attachment pre‑2010), make sure the belt is not broken!

The first step is to turn down the spindle speed with the Spindle Override pot while the program is running, but the slide is not moving. If necessary, set Spindle Off/Auto switch to Off, and turn the spindle by hand. (Alternatively, you can write a short program to see if any slide movement occurs). If movement begins at a much slower spindle speed, then the issue is with either the spindle encoder or the "opto‑isolators" on the MC2 board.

Check the encoder cable. Whether the slide begins to move at much slower spindle speed or not, unplug the encoder cable, examine all the pins for any irregularity, then spray the connectors with contact cleaner or alcohol. Belt‑driven encoderBelt‑driven encoder on Attachment cables have connectors on both ends; direct‑drive encodersDirect‑drive encoder have connector only at CNC control.
Re‑plug the connnectors and run your program; if the program runs, you've fixed the issue by cleaning the connectors.

If movement begins at a much slower spindle speed, it is very difficult to determine if the issue is with the encoder or with the optos. Replace the encoder first, and if that doesn't fix the issue, replace the optos.

If movement does NOT begin, regardless of spindle speed it is necessary to troubleshoot by moving the spindle encoder to the z‑axis input as described directly below.

To troubleshoot by moving the Spindle connector:

If no slide movement at any spindle speed, this proceedure will help determine if issue is with encoder or with opto‑isolators on MC2 card.

• Turn off the CNC
• Disconnect the Z‑Axis cable at the rear of the CNC
  
• Move the Spindle connector to the Z‑axis connection
  
• Turn on the CNC and turn on servos, but do not establish home.
• Go to Jog Mode, the press Ctrl‑E (Press and hold the Ctrl key, then press the E key) to open the following error display. You will first test for encoder counts, then for the "marker pulse".
  
• Slowly turn the spindle while watching the Z: encoder count.

  Turn the spindle slowly first one way, then the other less than 1/8 turn: the numbers should count up in one direction and count down in the other. NOTE: If you exceed 4000 counts, the servos will shut off.

• If the numbers don’t change, replace the encoder. NOTE: If you haven't already checked the cable, do it now.
• If the numbers increase and decrease, press Esc to exit Ctrl‑E. Jog the X‑axis away from home, then press 9, then Cycle Start to establish home. The screen will display "Z reference in progress".
• Slowly turn the spindle, up to one full turn, until the screen prompt changes to "X reference in progress" and the x‑axis moves toward home.
• If you can turn the spindle more than one full turn without seeing the prompt change and the X‑axis move, replace the encoder. NOTE: If you haven't already checked the cable, do it now.
• If the prompt does change, and the x‑axis moves to home, then the opto‑isolator inputs on the motion card (MC2) may be faulty.
• Turn off CNC and reconnect Z‑axis and Spindle connectors.

---

To troubleshoot by writing a short program:

(This method is alternative to turning down the Spindle Override pot while running your existing program, above).

• Write a program to move the z-axis one inch from home with one revolution of the spindle, starting the move at the "marker pulse":
g90g72g94f300
g95f1z-1p
m30

(The "P" at the end of the g95 block is to tell the slide to start moving when the spindle "marker pulse" occurs).

• Press Cycle Start, then turn the spindle slowly by hand, and verify that the z-axis begins moving minus at some point (this is where the "marker pulse" occurs), then moves one inch as you continue to turn the spindle one complete revolution past that point.