Program Stops

[Smit]

Can somebody please tell me how to force an output of a program stop at the end of a operation, retract the tool and then restart with the same tool. Ex. Mill one side of a part, program stop to move clamps, then restart with the same tool in the spindle? I've been doing it manually, and I've read several references to doing this. Any help would be appreciated.

Thanks,

Larry

[Allan Brown]

Download the 'Mpmaster' post from this site and use Misc Value, Misc Integer 10 set to 1 in second op.

# mi10 - M00 before operation

# 0 = No

# 1 = Yes

[Reece L Gibson]

Modify your own post

[Michael Reynolds]

Hi Larry! You could also try the "canned text" option in the tool parameters page. That will also force moo, mo1, m5, yada yada yada into your program. Might be easier than modifying your post.

Hope this helps!

Mike R.

[Mark H]

All you may need to do is select "force tool change" check box. Go to the Tools parameters tab, then "Change NCI" button. My post had this feature built into it. At the end of an operation the machine will go home in Z, shut off the coolant and stop the spindle, and wait for the user to hit cycle start button. And for this to work, I must select "optional stop ON" on my controler. Also with the machines here, I can not move any of the axis. (So indicating a part straight may be a problem, but you can get around this by having a vise and stops or some other similar setup)

BTW, I use this all the time to check the inserts on my endmills. I will replace them if they get too beat up. Of course I can't measure them in this mode, but the tool height usually stays the same (within .001).

[kathy]

Hi,

I have a pstop sequence in my Fadal & Fanuc (Komo) posts that I tag with using Misc Variable 10. If I want to stop a tool between contours, I break the contours into a definate start / stop, and place a point on the start of the second contour. In the point's parameters, I eval MV 10 = 1. This inserts a pstop sequence (retracts and stops tool, moves table forward to home, and will add the tool start stuff after pstop) from my post(example Fadal):

pstop # program stop

n, "G00 G49 M47 Z0 M5", e

n, "E0 X0 Y0", e

n, "M00( PROGRAM STOP)", e

pss, e

n, "E1", *xr, *yr, e

n, ptllncomp,e

mi10=0

I also use a similar sequence when p-stoping at a tool change.

Kathy

[Rory]

I am running a Dynapath post.

In the post I set up the following line at

ptlchg

if mi2 = 1, n, "(9)M00", e

I am using Misc Integer 2.

1 = on, 2 = off

I also edited the text file that goes with the post.

Now when I set mi2 to 1 and use the force tool change option as Mark mentioned, the machine sends the spindle home and out puts the M00 program stop.

I am happy this question came up because I have been wondering about the same thing.

Rory

[HEAVY METAL]

THE FOREC TO CHANGE WORKS GREAT,BUT STILL OUTPUTS AN AT EVERY DEPTH OF CUT OR PASS.I.M I MISSING SOMETHING HERE

 

 

THANKS HEAVY

[Allan Brown]

The tool change at every depth when forcing the toolchange is a logged bug.