0TC Unexpected action

[alphonso]

0TC
Running program using G71 canned cycle and G70 for finish path.

Cut a little oversize. Wanted to just run the G70 cycle to see if it would clean up to size.

Block deleted both G71 lines and away we go. Ran the G70 just fine until it got to the end of the profile. Instead of returning to the start point it tried to send the tool to X zero or some such (program check button has quit working so I don't know where it was headed). Needless to say, not what I was expecting. Destroyed tool and knocked turret out of whack. Might take all day to get turret back.

Any idea why???


N10 T0202(DNMG 432)
M57
N20 M41
N30 G97 S618 M3
N40 G0 X2.1625 Z26.1
N50 M8
N60 G96 S350
/N70 G71 U.05 R.05
/N80 G71 P90 Q230 U.015 W.005 F0.015
N90 G0 X0.626
N100 G1 Z26.0
N110 X0.746 Z25.94
N120 Z24.9375
N130 G2 X0.871 Z24.875 I0.0625 K0.0
N140 G1 X1.19
N150 X1.25 Z24.845
N160 Z24.0
N170 X1.5 Z22.75
N180 Z22.1875
N190 G2 X1.75 Z22.0625 I0.125 K0.0
N200 G1 X1.94
N210 X2.0 Z22.0325
N220 Z21.7188
N230 X2.0625 <---------------------point where tool plunged toward X zero? instead of up and back to start point
N240 G70 P90 Q230 F0.01
N250 G97 S150
N260 T0200 M09
N270 G0 X11.7312 Z26.125
N280 M01

 

[lobust]

Where did you start it from to run the G70?

The start of the program or N240?

 

[alphonso]

Start of program. Positioned in N40, seemed normal until the tool went the wrong way.

According to Fanuc manual when G70 is finished the program is supposed to advance to the next block.

 

[lobust]

If you ran it from the start of the program, then you were not in G70.

It ran every line of code except N70 and N80, up until N240, where it jumped back to N90.

 

[alphonso]

Yeah, sitting on the throne this morning, I realized what happened. I guess I was thinking Fagor and GE 1050, where the profile is at the end of the program.

now to get turret back.

 

[mach ramsey mn]

Hey, it’s nice to see the update where the problem is figured out. Some of the threads here that go dormant without a resolution…

 

[Vancbiker]

Hey, it’s nice to see the update where the problem is figured out. Some of the threads here that go dormant without a resolution…

Sometimes folks figure out the problem was face palm worthy and therefore a bit embarrassed to admit.

 

[mach ramsey mn]

Right, sometimes even chuckle worthy! But if there is any of us here that hasn’t done that we are all liars!
I still like to hear the resolution as it might pop to my every failing memory when I fat finger something!
My favorite used to forget to get an end of block after an M30 and the program would just stall about 3-4 blocks before the end of the program… old 6m control, back in the day…

 

[Herding Cats]

program would just stall about 3-4 blocks before the end of the program…

Now that's some look ahead

 

[Vancbiker]

Another 6M thing was a long line followed with a comment. If the combined length exceeded a number of characters (that I don’t recall now) the control would usually go crazy. When you looked at the code including that line in an editor or on screen it looked fine except that it wrapped on the control screen between the comment brackets.

 

[Spruewell]

Why would you put a block delete in front of the G71 commands?

N10 T0202(DNMG 432)
M57
N20 M41
N30 G97 S618 M3
N40 G0 X2.1625 Z26.1
N50 M8
N60 G96 S350
/N70 G71 U.05 R.05
/N80 G71 P90 Q230 U.015 W.005 F0.015
N90 G0 X0.626
N100 G1 Z26.0
N110 X0.746 Z25.94
N120 Z24.9375
N130 G2 X0.871 Z24.875 I0.0625 K0.0
N140 G1 X1.19
N150 X1.25 Z24.845
N160 Z24.0
N170 X1.5 Z22.75
N180 Z22.1875
N190 G2 X1.75 Z22.0625 I0.125 K0.0
N200 G1 X1.94
N210 X2.0 Z22.0325
N220 Z21.7188
N230 X2.0625
-------------------Break up the tool path and add a move to safe position
G0 X2.1625 Z26.1
M01
------------------Option stop, then have the finish cycle stand alone.
T0202(DNMG 432)
M57
M41
G97 S618 M3
G0 X2.1625 Z26.1
M8
G96 S350

N240 G70 P90 Q230 F0.01
N250 G97 S150
N260 T0200 M09
N270 G0 X11.7312 Z26.125
N280 M01


This will give you the flexibility to change finish tools, check size before the finish pass, or re-run the finish pass without having to go through the roughing cycle. With a block delete in front of the G71, you are leaving the door open for a crash when you inadvertently leave block delete on. This simple change is much safer and will not add time to the program.

 

[alphonso]

Actually I had considered single blocking down to N60, popping out to edit, scrolling down to N240, back to auto and continue on. Wish I had done that now.

Have spent 7 hours trying to get turret aligned. Not done yet. Squared up without incident, BUT.................................. turret spun a bit. Sags some when bolts are loosened. Get it clocked, tighten bolts. Shit, it is off .010. Try again, and again, and again.

Sure that it doesn't help that two adjacent bolts heads are broken off. Make drill bushing, left hand drill. Bolts came out without any fuss. Now find some new bolts. Maybe tomorrow, My back hurts so much I can't stand up.

 

[mach ramsey mn]

No dowel or taper pins to align to?

 

[alphonso]

Gone before I got the machine. Never trusted pins to line up on the money. Turret spins, pins get bent, holes wallered out. Fuck that, just leave 'em out.

 

[Herding Cats]

Gone before I got the machine. Never trusted pins to line up on the money. Turret spins, pins get bent, holes wallered out. Fuck that, just leave 'em out.

I agree, I have them pulled on all my lathes. I'm of the mindset of during a crash I want things to move and dissipate energy rather than break.

 

[mach ramsey mn]

Back in the day I worked for a machine tool dealer. Upon Instal of new turning centers they checked the bolts for torque and pulled the pins. When they got “bumped” just break the bolts loose put the pins back in snug them down and go from there. Save a couple three hours realigning from what I’ve been told.

 

[Spruewell]

Were the bolts in your turret broken before, or did it happen in this crash? I've hit a machine pretty hard in the past, but never managed to break a bolt in the turret.
I had a Miyano with dual turrets. The turning tool was on the bottom turret and as I was editing the program, the final move was a rapid in X away from the part up close to the chuck. Unfortunately, I missed the minus sign on the rapid move and it sent the tool from X-1.75 to X2.0 as fast as it could through 303 stainless about 1/2" from the collet face. Almost made it... Took me about a day to re align the turret and spindle. Didn't break any bolts

Looking at your Z values, are you programming in absolute? Or is your part 26" long?

 

[alphonso]

Not sure when the bolts broke the heads off. Either before I got the machine or a long time ago.

Absolute. Part is 26" long. 6" swallowed up in chuck and spindle. Leaves about a 1/4 inch distance to home position.

 

[mach ramsey mn]

Maximized part capacity, I love it!!!

 

[Spruewell]

Hard to imagine a bump that far out from the spindle causing that much damage.