how do you release the spindle lock during a tool change?

I need to rotate the tool in the spindle when the program calls for a tool change, but Dialog has it locked.

I need to line up the tool bit after a boring pass, then move the tool head a few thou away from the tool bit before the boring head is retracted. This was a good suggestion made by Ross. It works fine in mode 7 but in mode 8 I can't find a way to release the spindle. I tried setting the speed to zero in the same block where the tool change is called, but it didn't help.I also tried using M00 instead of a tool change, no difference.

I guess if there is no way to do it, I can just reverse direction and bore the cylinder again on the way up, but that only solves half the problem (I still need to adjust the boring head for the next pass, which also uses a tool change, the way the program is currently written).

Another question I have related to boring: should I use M21 & M23 to lock the X&Y axes during boring in Z? Will it result in a more accurate bore?

-Dave

The way i do this is not use the boring cycle....That cycle returns the tool to the clearance plane as part of its canned cycle.

I program to the needed depth using "Z" or "Y" depending on the setup (vertical or horizontal)

At the bottom of the hole when the depth target is reached i do a speed change to S+ 0...that shifts the gearbox to neutral.
Then the next block i call an M00 which is a program stop...Machine will wait there till you push the cycle start again....
Here is where you manually orient the tool by hand .(spindle will rotate freely being in neutral)..
Then hit the cycle start and the program begins at the next block after the programmed stop.
Next line give the slide a small move in a direction that moves the cutting edge off the part slightly (remember that you clocked the tool when it stopped)
Now program your retract move as a rapid, and finally reposition the axis back to be on center with your part.....

Another advantage here is that the spindle will be in neutral so positioning to adjust your next move on the boring head is now easy....
I don't always use the programmed stop orient the tool or step off the part surface deal , but pretty much always use the neutral shift at the end of the cycle to make boring head adjustment easier....
Cheers Ross

Dave:
i re-read your post...Do not do a tool change to get the spindle to neutral ....Do a speed change at the bottom of the hole to S+0
Don't you want to be running in mode 9 ?

Code might look like this:

N1
G0
X0
Y0
Z4.0

N2
S+200

N3
G0
Z.1

N4
Z-4.5
F.8

N5
S+0

N6
M00

N7
G0
X.03

N8
G0
Z4.0

N9
G0
X0
Y0

N10
M30



Of course you need to fill in the specific D2 comp calls for length if you are using any (don't really need any for this job i believe)

Cheers Ross

Ross, thought I tried that combination, but I will try it again and report back.

Thanks, Ross. I figured it out. This works:

N005 S+0 M00

This doesn't (but Dialog accepts it as valid input and displays the speed without a sign):

N005 S0 M00

Actually using S0 is a habit I have fallen into, and it does work to set the speed to zero (stop the spindle), but it doesn't release the spindle. For whatever reason, S+0 sets the speed to zero and releases the spindle. I also tried it setting the speed to zero the prior block, before the M00, and the same holds true. Anyway, thanks for your help, I thought I had tried every combination. Note to anyone reading this, I am using D2, and I don't know if this applies to D3 or 4.

-Dave

Dave:
All Dialog controls (2-4) require a sign (+ -) as part of the speed call...
By programming "S0" you are simply stopping the spindle , there is no gear change .
No sign in the speed code and the control simply turns off the main drive motor leaving the gears engaged at the same ratio as it was programmed for in the last speed change.....
....its not seeing a speed "zero" rather it isn't seeing any speed at all.


Note:
On D4 the control will "accept" an entry of "S0" in fact that is the only numerical value that can be entered if no sign is used. Looks like the "S0" will call a spindle stop and can be used in a program
(not sure why one would want this) and you can resume the spindle by using another (proper) "S" call in the program.
However it looks like the control limits that do not allow feed motions without the spindle running still apply for the S0....Rapids do work however, and as a note...Feed motions do work under S+0....
Cheers Ross

The only reason I can think of for having S0 stop the spindle motor without disengaging the gears is that there is no delay when the spindle is restarted, if the speed is the same. Sometimes when the spindle is rotated after disengaging the gears, the gearbox takes a few attempts to attain gear mesh when the spindle is restarted.

I use the S0 to stop the spindle and an M9 in the block before a program is done and returning to the start position. This allows the work space to stop dripping before I do a part change and doesn't put extra air cutting hours on my spindle bearings.
Dave