Guided Deep Drilling cycle on Siemens 840d control

[mikebirdwell]

Hey all, I'm currently working on a pneumatic manifold part that requires some quite deep holes (5mm 30x diameter, at the worst) and wanted to use the Guided deep drilling operation in Fusion. I have my operation parameters set up how I'd like, pilot holes are good, but my current post for the Siemens control on our DMU 50 doesn't seem to recognize it, it just uses a normal drill cycle (spins up to the drilling rpm before its in the hole, then spins down afterwards?). Could anyone assist in patching that functionality in? Doesn't seem that Siemens has a cycle that is what I'm after, though I'd love to be proved wrong. I've attached the current post and the generated code I have for the operation (forum won't let me upload an mpf file, I've converted it to a txt).

Also, the post seems to export an extraneous Cycle 800 at the beginning of the program and before each tool with a different orientation. Can't seem to find where that's coming from. I can just remove it in the g-code, but if anyone with better eyes than I could spot it, that would be great.

[KrupalVala]

Hi @mikebirdwell ,

Could you please tell me what format you want from the Guided Gun drilling cycle?

You are getting the Cycle 800 at the beginning of the program and before each tool is because it is resetting/canceling the swivel modes.

Thanks,

[mikebirdwell]

Currently, I have used the chip breaking cycle with my retract and feed height set slightly above where I have pre drilled, I then hand code it to initially spin to 50 rpm, feeding slowly to the retract depth of the drill cycle. it spins up to speed right before the drill cycle starts, then spins down back to 50 when it goes to "retract" (still in the hole) then slowly feeds out.

Here's an example of what I hand edited, I just proved out today that it works though I still have to hand edit all 6 cycles every time I repost (there are no sequence numbers where I have hand edited, commented some explanation).

N10724 ; Drill 11.8mm Right Side BALLS DEEP
N10725 M1
N10726 T10 D1
N10727 M6
N10728 T11
N10729 CYCLE832()
S50 M3 ; spin slow
N10731 G55
N10732 CYCLE800(1,"DMG",0,39,0,0,0,0,-90,90,0,0,0,1)
N10733 G0 X0.3596 Y2.6084
N10734 G0 Z5.75
N10735 M7
N10736 G17
G01 Z2.1 F10. ; feed to retract height
S1646 ; spin to cutting speed
N10737 F5.35
N10738 MCALL CYCLE83(2.1, 2.0197, 0.035, -0.4648, , 1.5551, , 0, , , 1, 0, , 0.4646, 0.0093, 5, 0)
N10739 X0.3596 Y2.6084
N10740 MCALL
S50 ; spin down
G01 Z5.75 F10. ; feed out of hole
N10743 G0 SUPA Z-0.01 D0
G0 SUPA X-18. ; safety move
N10744 CYCLE800(1,"DMG",0,39,0,0,0,0,0,0,0,0,0,0)

Also, that extraneous Cycle 800 seems to be a non issue now. For some reason when our other programmer was working on it, it faulted out the machine and did some funky stuff, but I didn't have that problem. Thanks for looking though.

[KrupalVala]

Hi @mikebirdwell ,

I would suggest you use the Guided Deep Drilling cycle instead of the chip breaking cycle. You will get more controllers on cycle in Gun drilling.

Thanks,

[mikebirdwell]

Sorry for delayed response, had some rushed jobs. I suppose I should have clarified, I would like to use the "guided gun drilling" cycle but my post does not recognize it. I had used the chipbreaking cycle with heavy hand edits to make it work for the job that needed to get out. My original question was asking if anyone could assist me in adding to the post to allow for guided gun drilling cycles, would like for it to work as posted if at all possible. 

[KrupalVala]

HI @mikebirdwell ,

I Modified the post and getting the below output. Need to modified the post in multiple areas. But I have a question regarding the format. What will happen if you do drilling in a multiple-hole position with this format? Will this drilling format work fine in that situation?  

Thanks