G76 Bore shift question - Mori Seiki with Fanuc control

[Guest]

I am trying to use a G76 with a shift at the bottom of a bore but getting the tool to line up properly and then getting movement in the correct direction seems to be an issue.

 

This is something I don't normally use so I am kind of at a loss as to how it's supposed to actually function.

 

G76 Z-.502 Q.01 R.1 F5.0

 

What am I missing?

[ToolMan184]

John, Isnt G76 a canned threading cycle insted of a boring cycle?

[Guest]

On a lathe yes, on a mill no, bore with a shift

[Steve Zirtzman]

John,

Would you need a G98 or G99 on the same line?

[ToolMan184]

My bad, you said Mori, I assumed a lathe.

[Kannon]

I dont know if its comparable but in quick code in the Haas.

It asks me for a G98, or a G99 first.

G98 is "CANNED CYCLE INITIAL POINT RETURN"

and G99 is "CANNED CYCLE R PLANE RETURN".

after filling out quick code it shows the line formatt like this

G76 G99 Z-.502 Q..01 R.1 F5.

 

Dont know if this helps you much.

[Tim Johnson]

You need to set parameter 5101 to tell the control which direction you want the retract(Fanuc 18i). You'll need the parameter book to get chart. Our machines are set to retract in the y- direction which would be RD2 set to 1 and RD1 set to 1 in parameter 5101.

[Guest]

I do have those set as you describe Tim.

 

Is there a way to get your machine to stop in a certain position so that the y move is actually off the bore wall.?

 

I'm using a boring head so I cannot change the positioning of the tool but it stops out of position for the y move, thus gougues the wall.

[lowboy]

A tool also shifts at the bottom by specifying addresses I an J.

G98G76X1.Y1.Z-1.R.1I-.01J-.01F15.

I and J are Modal I=X J=Y

[Jack Mitchell]

I-.01 will shift -.01" in "X"

J-.01 will shift -.01" in "Y"

 

The critical thing is you must set the tool tip at a quadrant in your spindle, then use the shift variable of "I" or "J" using a positive or negative shift.

 

PS. Some controls allow a shift amount and direction within a parameter setting.

 

Regards, Jack

[Guest]

Thanks guys,

 

I'll give the IJ shifts a try

 

[?Mark]

John, I doubt I J will work with fanuc on a mori.

 

Your code looks good, here is my sample for a mori:

 

G76 G98 X... Y... Z-... R.1 Q.005 F1.

 

quote:

---

The critical thing is you must set the tool tip at a quadrant in your spindle,

---

+1

It's a must on our moris.

 

And if it still doesn't work, foolow up on Tim's suggestion and make sure parameters are correct.

 

[?Mark]

BTW on our vertical mori's the boring bar tip has to be facing toward "y-", so Q shift moves the tool in Y+ direction, away from the wall...

 

hth

[Kelly Burns]

T9 M6

M01

G0 G90 G54 X-42.7323 Y-33.1407 S130 M3

G43 H9 Z3.5

G98 G76 Z-1.25 R.1 Q.005 F7.7

G80

 

In a Haas you have to define what direction the "q" shift is and orient the spindle when loading your boring head. You define it it the machine parameters.

[Tim Johnson]

Parameter 5101 for the Fanuc 18i control in G17 mode;

 

Retract in x+ direction; RD2 set to 0, RD1 set to 0

 

Retract in x- direction; RD2 set to 0, RD1 set to 1

 

Retract in y+ direction; RD2 set to 1, RD1 set to 0

 

Retract in y- direction; RD2 set to 1, RD1 set to 1

[Guest]

Tim

 

Thnaks, that goes into the bookmars

 

That's not in the book

 

[Tim Johnson]

Sorry I took so long to respond. That's in the Parameter book (but hand written in my operator's manual).

[WWFCAM]

another alternative is to us M19 to orient the spindle, feed using G1 moves and a shift on the proper axis depending on the shift direction within the control, also check that your bar is set correctly in the cat holder, the dimple in the cat holder, if set wrong the bar will shift in the wrong direction and scratch the bore coming out

 

mtc

[WWFCAM]

we use the G76 cycle all the time, and if the bar is not oriented to the dimple in the cat holder, either scratch or crash either way bad news

also set the q.005 if clearance on bar to bore is small

 

hth