[nfrees114]

So I have a haas VF-2 and have a peck drill cycle (G83). I have to retract 1" between holes to clear the fixture toe clamps. well I am cutting 1" of air on every hole. I was just wondering if there was a way to modify the G code so that it would start at .1" and drill the hole but then between the holes it would retract to 1". Any help would be greatly appreciated!!

Thanks!!

-Nate

[Superman]

Usually an R value defines the start of the cycle, called the retract plane
the initial level is the Z plane the tool is at before processing the drill cycle

ie
G0 X0 Y0
Z2.0 ( initial level )
G83 Z-1.5 R0.1 Q0.2 F4.000 M98 ( rapids to Z0.1, feed to Z-1.5, rapid retract to Z2.)
XY
XY M99 --> stays down( rapids to Z0.1, feed to Z-1.5, rapid retract to Z0.1 )
XY --> stays down
XY --> stays down
XY M98 --> goto Z2 at cycle end
XY


M98 is to return to the initail level ---being Z2.0, to clear all after each hole
M99 would make it go to Z0.1 after each hole --which would put you thru the clamps

You can put the M code after each hole to cut out the high retracts, but prove it off 1st without the clamps. The M code is modal.

[nfrees114]

So for this line of code I would change N132 line the Z to 1.0 not .1? and then on N133 give it a G98 code instead of a G99 code? and that will fix my problem??

(NEXT CUT - NEXT TOOL)
(JOB 4 HOLE RANDOM POINT PATTERN)
(3/16 HOLE)

N130 T03 M06
N131 G90 G54 X5.468 Y2.062 S3340 M03
N132 G43 H03 Z.1 M08
N133 G83 G99 X5.468 Y2.062 Z-.575 R.1 Q.0938 P0. F15.
N134 X8.468
N135 X11.468
N136 X14.468
N137 X17.468
N138 X20.468
N139 X23.468
N140 M09
N141 M05
N142 G00 G91 G28 Z0.
N143 M01

[nfrees114]

So for this line of code I would change N132 line the Z to 1.0 not .1? and then on N133 give it a G98 code instead of a G99 code? and that will fix my problem??

(NEXT CUT - NEXT TOOL)
(JOB 4 HOLE RANDOM POINT PATTERN)
(3/16 HOLE)

N130 T03 M06
N131 G90 G54 X5.468 Y2.062 S3340 M03
N132 G43 H03 Z.1 M08
N133 G83 G99 X5.468 Y2.062 Z-.575 R.1 Q.0938 P0. F15.
N134 X8.468
N135 X11.468
N136 X14.468
N137 X17.468
N138 X20.468
N139 X23.468
N140 M09
N141 M05
N142 G00 G91 G28 Z0.
N143 M01

Usually an R value defines the start of the cycle, called the retract plane
the initial level is the Z plane the tool is at before processing the drill cycle

ie
G0 X0 Y0
Z2.0 ( initial level )
G83 Z-1.5 R0.1 Q0.2 F4.000 M98 ( rapids to Z0.1, feed to Z-1.5, rapid retract to Z2.)
XY
XY M99 --> stays down( rapids to Z0.1, feed to Z-1.5, rapid retract to Z0.1 )
XY --> stays down
XY --> stays down
XY M98 --> goto Z2 at cycle end
XY


M98 is to return to the initail level ---being Z2.0, to clear all after each hole
M99 would make it go to Z0.1 after each hole --which would put you thru the clamps

You can put the M code after each hole to cut out the high retracts, but prove it off 1st without the clamps. The M code is modal.

[Superman]

Yep
Sorry, it should have been G-code G98/G99

put a higher figure in on N132, so you can actually see the moves, and miss the clamps, even if it had a nut/stud above the clamp

The P is a dwell, (in seconds) ---not necessary if a zero time, so it can be omitted

another trick use incremental

N133 G83 G99 X5.468 Y2.062 Z-.575 R.1 Q.0938 P0. F15.
N134 G91 X3.
N135 X3.
N136 X3.
N137 X3.
N138 X3.
N139 X3.
G90 ( to set back to absolute )
G0 (or G80 will terminate the drillcycle)
G94 ( force feed/min )
N140 M09
N141 M05
N142 G00 G91 G28 Z0.

G94 should be stated before a toolchange, just in case you copy & paste and change it to a tap cycle and use a feed/rev (G95) in it. The next toolpath would travel very quick.

[Geof]

I am puzzled. My Haas Manual says M98 is Sub Program Call and M99 Sub Program Return or Loop. Possibly you mean G98 Canned Cycle Initial Poibt Return and G99 Canned Cycle R Plane Return.

When there are obstructions you should use G98 and set the Z position ahead of the drill cycle high enough to clear them and set R just above the work. The drill cycle will rapid down to R, peck the hole retracting to R and then return to the Z position before moving to the next hole.