Fanuc 16-M -> won't feed when spindle is keylocked

[pwilson101]

We have a horizontal machining center with a Fanuc Series 16-M control. We need to back-chamfer (plunge) a hole, so we keylock the spindle, position in X & Y so we can feed through the hole, we feed in the Z-axis through the hole to get to the back, then we want to feed to the centerline in the Y-axis, start the spindle, feed in the Z-axis to desired depth, then reverse the process to get out of the hole.

The machine feeds no problem in the Z-axis with the spindle keylocked, but won't move in the X or Y-axis. Is there a parameter I need to change? Or is there another way to get through this? I'm stuck and the machine is down any help is very much appreciated...

Thanks

[dcoupar]

Have you tried the G87 Back Boring Cycle?

[pwilson101]

No I haven't tried the G87 cycle although that is probably a good idea.

What I did was change it to rapid (G0) instead of feed (G1) and it worked.

[dcoupar]

No I haven't tried the G87 cycle although that is probably a good idea.

What I did was change it to rapid (G0) instead of feed (G1) and it worked.

You didn't specify the machine make, but I know on some Doosan's/Daewoo's they have an M-code to allow it to feed with the spindle stopped. Maybe this is the case with your machine?

[underthetire]

Might try with a M19 as well.

[pwilson101]

It is a Daewoo...so there may be an M-code for feeding with no spindle? I have no M-code list for this machine, does anyone know what I can try?

And I tried it with the M19 and it didn't work.

[dcoupar]

It is a Daewoo...so there may be an M-code for feeding with no spindle? I have no M-code list for this machine, does anyone know what I can try?

And I tried it with the M19 and it didn't work.

What is the Model and serial number?

[dcoupar]

You might try M84. That's the code for a DHC400, anyway.

[ben_heinman]

Some machines have a keep relay for monitoring M3/M4 basically to check if the spindle is running during a feed (G01). Do you have a list of keep relays?

[drdos]

I just ran across this very same problem. What I found to fix this is parameter 3708 bit 0. Turn off bit 0 (xxxxxxx0)

[weibelmarco]

M84 will let you feed when spindle is stoped !
M85,M30 or 'Reset' cancels it

[dcoupar]

I just ran across this very same problem. What I found to fix this is parameter 3708 bit 0. Turn off bit 0 (xxxxxxx0)

Is your machine a Daewoo or Doosan?