G70 exit commands with a -u.

[rapidtraverse]

Hi there,

I experienced undesirable results while boring ,using machining cycle G71 and G70, and was wondering (WTF) how to correct my error.

After the G71 successfully completed a bore cycle with G41 in the P and Q; the g70 rapided the tool while still in, causing a crash!

The code looked fine. Matter of fact I copied the profile code and used this code and no g70 to finish machining the part with no crash.

Any ideas as to why this crashed?

Best regards,

Chris

[Geof]

You should post your code, that will make it easier to diagnose your problem.

My quick guess is that you were missing a G01 command in the P Q block. The G71 reads the feedrate included in the G71 line but the G70 reads the feedrate in the P Q block.

Post your code and I will run it through my simulator.

[Wiseco]

Like Geof said, it's probably a feedrate problem but post the code and we will help you.

[rapidtraverse]

Okay, here is my simple line of code in which the tool appears to rapid to g28 while stil in the part.

Thank you in adavnce.

Spindle stuff
G0 X.575 Z.1
G71 P23 Q30 U-.01 K.005 D.04 F.006
N23 G0G41 X2.1
G1 X1.415 Z0 F.003
X1.375 Z-.02
Z-2.0
X.937
X.875 Z-2.0312
Z-2.375
N30 G40 X.6
Z.1
X2.1Z.1
G70 P23 Q30
G0Z.1
G28
M1

[Geof]

Originally Posted by rapidtraverse Okay, here is my simple line of code in which the tool appears to rapid to g28 while stil in the part. Thank you in adavnce. Spindle stuff G0 X.575 Z.1 G71 P23 Q30 U-.01 K.005 D.04 F.006 N23 G0G41 X2.1 G1 X1.415 Z0 F.003 X1.375 Z-.02 Z-2.0 X.937 X.875 Z-2.0312 Z-2.375 N30 G40 X.6 Z.1 X2.1Z.1 G70 P23 Q30 G0Z.1 G28 M1

I ran it through my simulator and yes it went to the bottom of the hole and did the G28 from there. I can just imagine the crunching noise when this happens with a tool in a real part.

Then I deleted the two lines I made bold; the ones between your N30 and the G70 and it worked fine.

[swain]

I can check in the morning on my machine, But i believe the programmed path should have a g00 rapid to z.1 at the end before the g70 line. That makes it rapid in Z to clear the tool from the part. Let us know if geof got your problem solved or if you need me to, I can put the code om may machine and try it dryrun with no tool and nothing in the chuck. Let us know...good luck

Dan

[Geof]

Nothing is needed between the Q line and the G70. After doing the G71 sequence the machine returns to the starting point for the G71, which is G0 X.575 Z.1, then the G70 goes through the P,Q, block from there. The G70 picks up the feedrate specified in the P,Q, block and follows the programmed coordinates removing the finish allowance that was specified in the U and K for the G71.

The problem was the two lines I removed, the program ran correctly with them taken out. But why they should cause the machine to go to the bottom of the hole then do the G28 from there is a puzzle. Step through the two versions using Graphics and you will see what is happening.

[rapidtraverse]

Thanks Geof,

It's all comming back. Some time ago, as I recall, I was in a lecture about G71. They mentioned something about prep commands.

Thank's for your assistance.

By the way, carbide boring bars just kinda "POP!" Not really a crunch.

Chris

[Geof]

Originally Posted by rapidtraverse .....By the way, carbide boring bars just kinda "POP!" Not really a crunch. Chris

I did something similar years ago with an insert boring bar; they do not just 'pop'. There was an awful crunch and a whole lot of grinding noise until the Z servo overloaded and tripped an alarm.

[rapidtraverse]

Oh yeah, I've heard of such stories in a time before carbide boring bars.

Thanks again Geof

[Donkey Hotey]

Okay, I'm going to semi-hijack this thread since I just did the same type of operation.

I was making a hollow spindle out of aluminum. It had holes in each end but I was backboring inside to reduce weight. The trick was to put the boring bar through the hole, do a G71, then get it back out of the hole.

(Hollow inside cavity 1.9 deep) G71 P5 Q6 U-0.004 K0.002 D0.01 F0.003 N5 (Inside profile) G00 X0.97 Z0.2 (outside of hole) G01 X0.976 Z-0.2 F0.002 X1.196 Z-0.824 Z-1.9 X0.95 (I wanted this to be 0.750 but it seemed to have a problem with it) N6 G70 P5 Q6 G00 Z5. X0.82

I'm still a little shaky on the whole use of G71 inside a hole. Can somebody explain:

How did it determine to retract in the negative direction instead of positive (away from c/l)? I really wanted to guide it to a safe X diameter before retracting out of the hole but it was giving me fits (some kind of travel error).

I think it was due to the retract setting in the control (default) but I'm not sure. I think the original D value of 0.025" was too much. I'm guessing that with the start and finish diameters, plus the multiple of D, it couldn't retract safely and it knew it. But I'm not clear on it and that bothers me.

[Geof]

I will try to help with a few words.

Your "safe X" more or less has to be your starting X on the line immediately preceding the G71 line. For a hole all your other X coordinates have to be at a larger diameter. (For ODs of course all the others have to be smaller.)

Same thing with the Z on the preceding line to the G71. If you start at the outer end of your part all the Z coordinates have to be more negative; start at the inner end and they all have to be more positive.

The tool will always return to the starting X and Z and this is where the retract can have an effect. If you are in a tight bore the retract will sometimes take the boring bar into the opposite side. Go into the settings and make this retract no more than .01.

In addition don't make the X to much smaller for ID work or too much larger for OD than your largest, or smallest, final X dimension.

EDIT: Do you have a print? I could try writing the routine for what you are doing.


SECOND EDIT: Was your "travel error" something like 'Stroke Exceeded'? The error message when you have a move inside the P, Q, block that goes beyond the limits of your start position mentions something like this.