OSP7000 canned drillng with G127 plane change

[mkd]

I'm struggling getting fanuc type G98/G99 behavior contained in the canned cycle. So far i get no clearance plane retracts without programming rapids and a canned cycle for each hole.

 Any suggestions?

thanks in advance

(  LTR. A DRILL )
N130 MT=7603.
M321
G21HP=1
MT=3303.
M403
SB=1142 G52 TL=7676 BA=90.
M404
M110
G21  HP=4
G138 Y0.
M146
G00 C180.
M147
M13
G127 B90.
G17
G00 X-.6713 Y.879 M15
G00 Z4.
G00 Z3.
G00 Z.547
G94 G183 X-.6713 Z-.4173 C180. K.3 D.15 L.1 M08 F3.

****rapids straight accross****

X-7.0463
G180
*****need a g00 Z3. Here to keep g136 from crashing through the part****

G126
G136
X3000
G21HP=1
M12
M9
M01

[mkd]

i also tried this and got the same rapid above the hole behavior.

G00 X-.6713 Y.879 M15
G00 Z4.
G00 Z3.
G00 (Z.547)
G94 G183 X-.6713 Z-.4173 C180. K2.753 D.15 L.1 M08 F3.

****still rapids straight across****

X-7.0463
G180

[Mr. M]

I had to force canned cycles for each position on the P200 IIRC

[mkd]

ok, thanks for the tip.

I'll get the post tweaked that way.

just didn't want to have many canned cycles if there was a trick out there

[jeff]

Does your lathe support G71 and M53? Or is that just for mills.

 

G71Z2.
G83X-1.187Y0.Z-1.1573R.1Q.2F22.4M53
G80M54

[mkd]

Does your lathe support G71 and M53? Or is that just for mills.

 

G71Z2.

G83X-1.187Y0.Z-1.1573R.1Q.2F22.4M53

G80M54

Hmm...

as far as I know with plane change g127 active, the only supported canned cycles are three digit G/181/183/etc

 

 

G71 is a threading cycle and M53 is some gripper function/option.

I'm guessing there is some trickery available without using plane change and going the G17/G18/G19 route...

[Mick]

Is this on a MacTurn? Just curious.  From memory, The I and K values control the rapid depth, and it is a case of always programming to highest clearance point, and then using the I/K values to control the point in which the tool rapids to the start of feed.

 

I'd have to revisit it, as I haven't programmed the Multus with Mastercam in a while.

[jeff]

Hmm...

as far as I know with plane change g127 active, the only supported canned cycles are three digit G/181/183/etc

 

 

G71 is a threading cycle and M53 is some gripper function/option.

I'm guessing there is some trickery available without using plane change and going the G17/G18/G19 route...

Oh yeah, I forgot that G71 would be a totally different code on a lathe. 

 

That code snippet is for my osp300m

[mkd]

Is this on a MacTurn? Just curious.  From memory, The I and K values control the rapid depth, and it is a case of always programming to highest clearance point, and then using the I/K values to control the point in which the tool rapids to the start of feed.

 

I'd have to revisit it, as I haven't programmed the Multus with Mastercam in a while.

BINGO

Macturn30

 

 

G183 Deep Hole Drilling Cycle

(With repeat function)

 

G183, X, Z, C, R,

I(K), F, Q, D, E, L

 

E100L manual the Brad got me has this excerpt.^^^

 the I/K are incremental depths sown to the "R" plane for face/radial cycles. not sure how that matters with G127....K works all over.

 

my post guy got me a revision to issue a canned cycle for each hole. not elegant, but if it works...