Thread: Fanuc OT-C

Hi Guys


I have a problem with a Daewoo Puma 8S with a Fanuc OT-C control, I have been trying to thread on this for some time, every time that I have tried the tool will not follow the same path twice. The RPM shows on the screen so I think the encoder is good. Is there some parameter that controls when this tool should start in the right timing.


Thanks for your time and help, I really need it this has been on going for months.


Mike Roy In Canada

The spindle encoder does two things. It provides a stream of pulses so the Z axis can move at the same thread pitch even when the spindle RPM may vary a bit. These same pulses are used for the RPM display on your CRT. The other important function is from the "Zero" pulse, which is a single pulse every revolution of the encoder. The zero-pulse is what triggers the start of the Z motion in a threading cycle. Obviously, you're encoder is outputting a zero pulse, otherwise the CNC would just sit there waiting for it to begin the threading pass. Your problem seems to be that the zero pulse is not happening at the same spindle position each time.

Look for some slippage between the encoder and the spindle. Most encoders are belt driven, and the belts can wear. The pulleys can also slip if there is no keyway. If you can turn the encoder at all while holding the spindle stationary, you've found the problem.

Another thing you can do is program a threading cycle with a very slow spindle speed and a very fast pitch. You can then mark the chuck with a magic marker and see if the Z motion is starting at the same spindle angle each time while "threading air"

You ARE using a threading canned cycle, aren't you? I've seen some folks who've never threaded before simply program a bunch of Z motions and expect the machine to thread. Normal Z motions disregard the encoder zero pulse, so the Z motion would never start in the same place twice.

I suggest you use G76. It does all the work for you to generate multiple threading passes with a one block command. If you are using G76, be aware that each pass is NOT SUPPOSED to follow the exact same thread center each time. The "A" angle is intended to always cut with a chip on one side of the tool, so the "A" command in the G76 block should always match the angle of your threading tool. An "A" value of zero would have the tool just cut deeper and deeper with each pass, and it would be throwing a chip on both sides.

Your part's not slipping in the chuck or collet, is it ?

You're not using Constant Surface Speed, are you? As you make each threading pass, the X dimension changes. In CSS, the spindle speed would increase a little on each pass. This is bad, because the CNC takes a certain amount of time to react to that encoder's zero pulse, and the threading pass would shift in Z.

Be sure CSS is off. Most Fanucs use G97 to cancel CSS.

One other thing that can cause trouble is not starting far enough away from the part in Z. If you start each threading pass too close to the part, your Z servo will still be accelerating when the tool engages the part. The Z axis needs to be completely up to speed or there will be a bit of pitch error on the first thread or so. Starting about .100 inch away is usually enough.

You may want to check for backlash or fishtail when an axis reverses direction. This is usually a common problem. Here is a page that can explain this to you.
Machine tool backlash check procedure

Also some machines have just one prox switch that is used as a tac for spindle speed. Make sure it is cleaned and adjusted properly.