[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]

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]

.....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.

[SeymourDumore]

About the original question - not sure but will check it out in a bit - I believe the start point for the G70 must be the same as the G71.
In the example above, the G71 starts at X.575 Z.1, while the G70 is sent to X2.1 Z.1

Again, this is just a guess atthis point, will confirm.

Now, a couple questions for you fellas?

1: Do you normally use the roughing tool for finishing?

2: Since the P-Q blocks are the same for G70 and G71, how do you ever put in deburr radiuses or edgebreaks? How'bout inside corners with tight fillet callouts that are smaller than your roughing tool?

3: Why do you use U and K rather than U and W? I can see U W I K, all in one cycle, but U and K doesn't seem to make sense?

Just askin'....

[Donkey Hotey]

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.)

I think this was my problem. In the attached print, Z=0 was the face on the right of the part. You can see that the starting bore was larger than the finishing bore (the whole inside was turned from the right side of the print). I think the default retract distance in the control is 0.025 and that, plus my ending position of X.790 Z-1.90 was unable to retract away from the corner by 0.0250" It worked when I ended at X1.195, Z-1.190 but that meant I was unable to really finish the far, inside wall.

If I could have figured it all out, I would have done the entire inside bore with rounded corners (right out the other side of the part). But that meant that the profile started at X0.95 and ending at X0.790. What I wanted it to do was just end at X0.790, retract about 0.010 and rapid out of the hole.

The only solution I could come up with there would be to just program the path and not bother with G70,71,72.

SECOND EDIT: Was your "travel error" something like 'Stroke Exceeded'?

Yup, that was it.

[Geof]

About the original question - not sure but will check it out in a bit - I believe the start point for the G70 must be the same as the G71.
In the example above, the G71 starts at X.575 Z.1, while the G70 is sent to X2.1 Z.1

Again, this is just a guess atthis point, will confirm.

Now, a couple questions for you fellas?

1: Do you normally use the roughing tool for finishing?

2: Since the P-Q blocks are the same for G70 and G71, how do you ever put in deburr radiuses or edgebreaks? How'bout inside corners with tight fillet callouts that are smaller than your roughing tool?

3: Why do you use U and K rather than U and W? I can see U W I K, all in one cycle, but U and K doesn't seem to make sense?

Just askin'....

First Points:

Yes, G70 starts same place as G71. Regardless of what is the last command in the P, Q, block after the final run through in the G71, this is the run through where it steps through line by line, the machine will rapid from the final point in the P, Q, block directly to the original start point that is defined on the line ahead of the G71.

Copy the code and run it through Graphics. The two lines between the end of the P, Q, and the G70 might appear to send it to X2.1, Z.1 but in fact on my simulator the tool dived right to the bottom of the hole and then did the G28 from there. Taking these two lines out as I did removed this move but did not alter the P, Q, profile.

Question 1: Very often yes, but I am working with leaded steel or aluminum so having a separate finish tool is really not needed. Also my tolerances are generally quite sloppy, +/-0.001 very often.

Qestion 2: Then use a separate finish tool; but make sure you do not have a T in the G71 line because that overrides and tool change you put in the P, Q, block (I think that is correct).

Question 3: Because K and W are equivalent and optional; read the manual description.

[Geof]

......The only solution I could come up with there would be to just program the path and not bother with G70,71,72.

Yup, that was it.

If you can program the path you can do it using the canned cycles.

I will play around on my simulator this evening and tomorrow evening and see what I can come up with from your drawing.

[Donkey Hotey]

I forgot to add:

The part started out with a 1/2" drill hole, all the way through.
Then I bored 0.790 all the way through.
And another bore of 0.975", 1.900 deep.

That way, all I was left with was the back-bored cavity. I could have left finish allowance on the pre-bores but since I wasn't getting any love from G71, I gave up and just finished them to size in the first operations and left them alone. In fact, I ramped into the first point at X0.976 Z -0.2 (from a 'safe' diameter of X0.970).

And the reason for that goofy ramp angle is that's all my boring bar could do (10 degree back angle on the cutting edge).

Oh yeah: Geof, I've already made two of these and the remaining two will have to be largely the same. While it's greatly appreciated, don't spend a bunch of time trying to get me out of a pinch. The code I have is good enough for this one. I'm trying to understand and learn for 'next time'.

[Geof]

.....Oh yeah: Geof, I've already made two of these and the remaining two will have to be largely the same. While it's greatly appreciated, don't spend a bunch of time trying to get me out of a pinch. The code I have is good enough for this one. I'm trying to understand and learn for 'next time'.

In the evenings I normally have free time because I don't watch TV, more correctly I cannot stand to watch TV. I will see what I can fit in between reading the nespaper and knocking back a half a bottle of wine.

[SeymourDumore]

Geof

Remember, you've said that removing teh X/Z moves from the code corrected the problem?
In the original code:
N30 G40 X.6
Z.1 <---
X2.1Z.1 <---
G70 P23 Q30

The tool, after the end of N30 was put back to X.575 Z.1, which was the start point for the G71 cycle. The blocks marked with the arrows moved the tool to X2.1 Z.1, and the G70 cycle was called.
This is what I meant by G71 and G70 NOT starting from the same point. After the removal of those 2 blocks, the G70 started from the point where G71.

As far as W and K, nope, they are optional but NOT identical. W is finishing allowance, K is roughing allowance. It only exist in Haas, and is a wondeful thing.
Typically U and W is used, which creates a single pass at the end of the cycle. If I ank K is used in ADDITION to the U and W, you'll get 2 passes at the end of the cycle. The first one is offset by I and K, the second is by U and W.
I use it always when tight tolerances of the whole contour required, or when surface finish is critical.
For example, the code above would look like this:

G00 X.575 Z.1
G71 P23 Q30 U-.01 W.002 I-.015 K.005 D.04 F.006
N23 G00 G41 X2.1
G01 X1.415 Z0 F.003
G01 X1.375 Z-.02
G01 Z-2.0
G01 X.937
G01 X.875 Z-2.0312
G01 Z-2.375
N30 G01 G40 X.6
G28
M30

This creates 2 final passes between P and Q. One is X-.015/Z.005 away, the second is X-.01/Z.002 away.

[Donkey Hotey]

Dang, guys, I'm learning a lot from this thread. The WUKI options had me confused as well. Great explanation Seymour. Youz guyz should be writing for Haas.

I've had a few hours to let this discussion simmer:

The reason I was afraid of using a G71 move all the way through the profile was retract (X) clearance with the boring bar. If I tried to use G71 from outside the hole, my fear was that it would try to offset the first roughing pass to a smaller diameter than the bar had clearance for (0.5" bar in a 0.5" hole). If the bar tried to retract to a smaller diameter than 0.5", the backside would crash.

Would it be correct to say that the starting X,Z position, above the G71 block is assumed to be the outside of the actual material? Or inside in the case of a bore? And it uses the retract distance setting to retract from this imaginary material limit?

So using a G71 profile for a bore:

• If the starting position of the cutter (above the G71 line) was .600"
• Then the farthest the cutter will ever retract during that cycle will be X0.600 and the retract distance set in the control (X0.590" in the case of 0.010" retract setting)?
• And it will do the rapid retract in equal amounts (45 degree move) until each distance is reached? In other words, if a feature might be in the way, there needs to be extra X and Z travel for the rapid move away from the profile?