Custom Drill cycle

[JeremyV]

Would anyone know of a custom canned drill cycle that does exactly what it should do and not having to manually type in all the codes?

 

Here is what I want to do:

 

a combination of G83 and G73:   

 

Drill will start at ref z.1 plane then rapid in Z-1.3" to eliminate air cutting time in a pre-drilled hole.

 

Drill will start the G73 cycle for 1" then return to ref plane to clear chips then resume cutting from the previous spot at G73 for another inch and repeat till it achieves the 7" depth.

 

Make sense?

 

 

-JD

[absolute technologies]

We use a custom G-code macro at the machine called by a G183 but instead of rapiding into the pre-drilled hole it feeds into the hole at 4X the programmed federate or whatever you set it at. IMHO a G-Code macro at the machine gives us more flexibility than "building" the routine in MasterCam especially if you will need it on multiple jobs you only have to build the Macro once and get MasterCam to post a G183 with the necessary codes for it. Attached is some example macros, it doesn't do the G73 short peck type but that could be easily changed or added. It does let you drill down to a point prior to pecking and also you can specify where the drill pulls out to like for really long drills that would snap off if you pulled out of the hole with the spindle on something like .050 just inside the hole which also prevents the drill from clipping the edge of the hole each peck because your drill run-outs a bit.

 

Cheers!

Len DYe

 

 

 

 

Custom Drilling Macros.zip

[cncchipmaker]

O5000(G83 & G73 DRILL MACRO)
(ABSOLUTE MACRO)
(WORKS)
 
(FORMAT G65/G66 QRZEFIH)
(Q = #17 - STEPOVER IN Z/ DOC)
(R = #18 - R PLANE)
(Z = #26 - Z START ZERO)
(E = #8 - END OF DRILL IN Z)
(F = #9 - ENTRANCE FEEDRATE)
(I = #4 - PECK FEEDRATE)
(H = #11 - IN AND OUT FEEDRATE)
(*********************************)

#100=ABS[#26]-ABS[#8]
#100=ABS[#100]
IF[[#26*#8]GE0]GOTO1
#100=ABS[#26]+ABS[#8]
N1#101=ROUND[#100/#17]
#102=#100/#101
#103=#5001
#105=#5002
G0G90X#103Y#105
Z#18
G1Z#26F#9
#106=#5003
WHILE[#101GE0]DO1
IF[#101LT0]GOTO10
#101=#101-1.
G1Z#106F#4
Z#18F#11
Z[#106+.005]
#106=#106-#102
END1
N10G0G90Z#18
X#103Y#105
M99

 

Give this a try.

[JeremyV]

Thanks guys!

[crazy^millman]

We use a custom G-code macro at the machine called by a G183 but instead of rapiding into the pre-drilled hole it feeds into the hole at 4X the programmed federate or whatever you set it at. IMHO a G-Code macro at the machine gives us more flexibility than "building" the routine in MasterCam especially if you will need it on multiple jobs you only have to build the Macro once and get MasterCam to post a G183 with the necessary codes for it. Attached is some example macros, it doesn't do the G73 short peck type but that could be easily changed or added. It does let you drill down to a point prior to pecking and also you can specify where the drill pulls out to like for really long drills that would snap off if you pulled out of the hole with the spindle on something like .050 just inside the hole which also prevents the drill from clipping the edge of the hole each peck because your drill run-outs a bit.

 

Cheers!

Len DYe

 

Len, do you know how to adjust Mastercam to support and output those canned cycles for the Machines you are programming? In other words have these drilling cycles show up in the Mastercam drilling cycles with those letters defined and get output that makes the G182 and G283 cycles?

[absolute technologies]

Len, do you know how to adjust Mastercam to support and output those canned cycles for the Machines you are programming? In other words have these drilling cycles show up in the Mastercam drilling cycles with those letters defined and get output that makes the G182 and G283 cycles?

Ron

 

I've never bother setting up MCX to output all the variables for the G183 or G283 drilling cycles. Where I'm at now I might use it once a month if that and it's mostly when process improvements come along and the G-Code is all ready set. At my last place we ran mostly Oil Tool parts where the drill macros come in real handy thou but never bother setting up MCX there either. I imagine one would use a Custom Drill cycle, some standard settings and Misc. Values  to get the post to output all the variables needed. That's starting to get out of my league with programming with MCX thou.

 

Hah, I'm still using my heavily modified X5 post that's been converted when each new version comes out. When we get MC 2017 I'm finally going to break down and buy a new post more than likely thou.

 

Cheers!

Len Dye

[crazy^millman]

Ron

 

I've never bother setting up MCX to output all the variables for the G183 or G283 drilling cycles. Where I'm at now I might use it once a month if that and it's mostly when process improvements come along and the G-Code is all ready set. At my last place we ran mostly Oil Tool parts where the drill macros come in real handy thou but never bother setting up MCX there either. I imagine one would use a Custom Drill cycle, some standard settings and Misc. Values  to get the post to output all the variables needed. That's starting to get out of my league with programming with MCX thou.

 

Hah, I'm still using my heavily modified X5 post that's been converted when each new version comes out. When we get MC 2017 I'm finally going to break down and buy a new post more than likely thou.

 

Cheers!

Len Dye

 

Al easy stuff for what you are needing. Get a hold of CCCS they are about 5 minutes from you guys and they will get you going in the right direction.