Peck drilling cycle questions - G83/G83.6

[Springy]

Fanuc 0i control, trying to work out how to get a peck drilling cycle in our lathe that is defined as follows:

• Z0. is the surface plane of the part
• Any Z negative moves (eg Z-1.000) is inside the part boundary
• A slightly larger hole is predrilled to Z-1.000
• We want to rapid in close to Z-1.000 (say Z-0.950), drill to Z-2.000 and have a pecking depth of 0.100 but have the drill retract outside the part on each peck to remove chips

If I specify:
G0 Z-0.950 (rapid inside part that's already pre-drilled to Z-1.000 with a slightly larger diameter)
G83.6 Z-2.000 Q0.100 R1.000 F0.005
G80
G0 Z1.000 (rapid out of part)

What I get is the drill rapiding to Z-0.950, then rapiding back out to Z0.050 (that being the position defined by the R value), then starting to drill from there with pecks of 0.100, which saves me no time over simply sending the thing to Z0.050 and drilling from there.

Is there a way to have it rapid to the Z-0.950 starting point and actually start drilling from there without peck drilling an inch of air first, but also retracting back outside the part with each peck (and rapiding back to where material actually exists to be drilled after each retraction)? I've tried a number of combinations of G83/G83.6, starting points and R values but haven't managed to get it sorted.

 

[MaxPrairie]

G0 Z-0.950
G01 Z-1.1 F0.005
G0 Z.05
Z-1.08
G01 Z-1.2
G0 Z.05
Z-1.18
G01 Z-1.3
.
.
.
.

G0 Z1.000 (rapid out of part)

 

[Fancuku]

G0 Z-0.950
G01 Z-1.1 F0.005
G0 Z.05
Z-1.08
G01 Z-1.2
G0 Z.05
Z-1.18
G01 Z-1.3
.
.
.
.

G0 Z1.000 (rapid out of part)

Agree. This way will never fail you.

 

[SeymourDumore]

Funny thing is Haas has figured a way out of that some 30+ years ago by adding a setting called " CAN Cycle Retract Above R"

But
that
doesn't
help
you ....

 

[Springy]

G0 Z-0.950
G01 Z-1.1 F0.005
G0 Z.05
Z-1.08
G01 Z-1.2
G0 Z.05
Z-1.18
G01 Z-1.3
.
.
.
.

G0 Z1.000 (rapid out of part)

Thanks Max, however this is an issue we run into often enough now that we'd like to find a better way than hand-coding peck retracts. In some cases we'd have to manually write out hundreds of lines of code to do so, it's just not feasible because if/when we find we want to play with the pecking depth or feed rate, all of a sudden we've got another hour of rewriting it.

 

[rcs60]

this is fanuc programming
If your machine has macro ability it works well



#501=.100(R PLANE)
#502=-.400(STARTING PECK)
#503=-1.830(FINAL DEPTH)
#504=.100(PECK INCREMENT)


WHILE[#502GT#503]DO1
#505=[#502-#504]
IF[#505LT#503]THEN#505=#503
G0Z[#502+.05]
G1Z[#505]F8.
G0Z[#501]
#502=#502-#504
END1

 

[MaxPrairie]

Thanks Max, however this is an issue we run into often enough now that we'd like to find a better way than hand-coding peck retracts. In some cases we'd have to manually write out hundreds of lines of code to do so, it's just not feasible because if/when we find we want to play with the pecking depth or feed rate, all of a sudden we've got another hour of rewriting it.

Ahh okay. Here is a program for tsc drill.

G0 Z-0.950
G01 Z-2.0 F.005
G0 Z0.1

 

[andrew.grossi@biochemflui]

WHAT IS THE DEPTH OF Q2000 PECK VALUE IN A CNC MILL/TURN LATHE PROGRAM?
THANKS!

 

[angelw]

WHAT IS THE DEPTH OF Q2000 PECK VALUE IN A CNC MILL/TURN LATHE PROGRAM?
THANKS!

If the control was in G20 Mode Q would equal 0.2". If in G21 Mode, then Q would equal 2.0mm

Regards,

Bill