Program Stops With Spindle Running (G4 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).

The next step, whether or not the slide begins to move at much slower spindle speed, is to 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.

Verify that the progam is stopped at a g95 block, usually right after a tool call. If this is the case, then troubleshoot the issue using the Ctrl-S diagnostic as follows:

• Go to Jog Mode
• Press and hold the Ctrl key, then press the "S" key (Ctrl-S)
• You should see a star (*) to the right of RPM in the spindle speed box. The number to the left of RPM is encoder counts:
  

  Turning the spindle by hand will increase or decrease the numbers until the marker is encountered. There are 4000 encoder counts and one marker. When the number increases to 3999, the marker is encountered, then the number resets to zero.

• Slowly turn the spindle while watching the encoder count.

  Initially, turn the spindle first one way, then the other less than 1/8 turn: unless you are right at the marker, the numbers should count up in one direction and count down in the other.

• If the numbers don’t change, or if they only change in one direction, the encoder, or the encoder cable could be faulty. First check the cable. If it's a belt-driven encoderBelt-driven encoder on Attachment, unplug both ends and examine the contacts. If it's a direct‑drive encoderDirect-drive encoder the cable has only one connector, at the CNC. Examine pins for any obvious damage, then spray with contact cleaner or rubbing alcohol, re-plug and test again. If the problem persists, then replace the encoder.

• If the numbers increase and decrease, turn the spindle to increase the numbers. If the marker is working properly, the numbers should count to 4000, then start over at zero. If the numbers don’t reset, the encoder, or the encoder cable could be faulty. First check the cable. If it's a belt-driven encoder, unplug both ends and examine the contacts. Direct-Drive Encoder cables have only one connector, at the CNC. Examine pins for any obvious damage, then spray with contact cleaner or rubbing alcohol, re-plug and test again. If the problem persists, then replace the encoder.
• To cancel Ctrl-S press Ctrl-S again.

---

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.

---