O/T - Okuma Horiz. G76

[Randy Morton @ Clem Industrial]

Hey,

 

I have the OSP E100M control on my Okuma Horizontal. MCX spits out the code just as described in the programming book...

 

G71 Z2.

G76 Xxx Zxx R.25 Q.05 F10. M53

 

When it comes to this line it gives me an alarm saying that there is no shift value or the shift value is wrong. It shows in the book and the on screen help that Q, I & J are the allowable varbiables, but it won't accept it.

What's the deal?

[jeff]

I don't know, it looks fine to me.

Have you used the G76 on that machine before?

Is that an option?

Try an I/J value instead of a Q.

That's all I got.

[Randy Morton @ Clem Industrial]

I haven't used it before. Machine is still getting the shipping dust off it.

 

The book says I&J are for the other planes (G18,G19)...

 

I'll just keep trying for now, but thanks for the input, Jeff!

[jeff]

You're welcome

[Jean-Simon]

Many Okumas here and in the g83, we're outputting I and J's in G17. Let's say I=0.05 J=0.200, it would chip break every 0.05 and do a full retract every 4 chip break. Is your Z2. value higher then your drilling depth? And last thing, here I put my m53 on the same line then G71. Feel free to e-mail me. I did'nt have time right now to put it in a machine and see but tomorrow, will give it a try.HTH!

 

Simon

[Rick Henrickson The Boeing Co.]

G76 is a fine boring cycle

bores in stops orients shifts off and rapids out

[jeff]

Jean-Simon

I have my M53 on the same line as he does and mine works fine.

G81 and G83 does, I never used the G76 yet

[Rick Henrickson The Boeing Co.]

note you have to have the bore tip oriented in x or y for your offset

 

Boring fixed cycles

 

G76 fine boring fixed cycle

Refer to drawings on the next several pages G76

 

EXAMPLE

G17 G40 G80 G90 G94

G15 H1

G00 X0 Y0 G56 H1 S1200 M03

Z0.1 M08

G95 F0.0015

G76 Z-1.0 R0.1 J-0.005

G80 G94 M09

G00 Z50

Y50

M02

 

EXPLANATION

G76 cycle requires an X and Y location either in the line or previous. A Z depth Z –1.000 (bottom of hole). Feed rate is specified in G95 inches per revolution or G94 inches per minute, a return plane R0.1

 

Machine positions tool to X and Y coordinate

Turns spindle on clockwise

Feeds down to the Z value specified

Spindle stops moves away from bore specified by the I and/or J value

Rapids back up to the R plane

Then turns the spindle on again to the clockwise direction.

 

Note: the I and J value needed to offset the tool from the bore are dependent on the way you orient the bar in the holder, and where your specific machine orients the spindle. The best way to find out where your spindle orients is to manually orient the spindle from the control panel. Then decide how you are going to locate your boring bars in the holders.

 

Refer to the drawing on the second page ORIENT

[chris m]

Randy, in the older OSP controls the shift direction was defined by a parameter when programming with the Q word; is it possible this parameter is not set so the machine doesn't know which way to go? It is also possible that there is a maximum value for Q and you've exceeded it, but I doubt that.

 

We back-bore all the time with G87 and the M53 is fine on that line, BTW.

[Rick Henrickson The Boeing Co.]

another cool thing for peck drilling is change of rough cut conditions

 

if you want to peck every .25 until 1 inch deep you can change the pech to .125 up to 2 inch deep and so on

 

after g83 line x y r z etc add

ZA=depth to take affect QA= new chip break

then ZB = QB =

etc

oh and FA to change feed to