What's new
What's new

HAAS ST30 canned cycle issues

AirLakeMachine

Plastic
Joined
May 17, 2017
Hey guys,

So here is the issue. while running parts with a canned cycle using cutter comp(G42/G41) my dimensions will come out different than when not using C.C. im not talking the small bit that should be expected but .03 worth of material, both on X and Z. I'm wondering if there is a setting or PARA that might be goofed. i touch everything off old school, without the probe, so i dont think the probe has anything to do with it but havent completely ruled it out. I dont use the probe because it is .3 off on z even after going through the calibration process, i can get X+ to cut to size with it however. Thats for another thread at a later time though. For now if anyone has insight on this issue it would be greatly appreciated.
 
Your insert has a .030 radius?
You're using your comp backwards.



Using comp backwards??? i wasn't aware this is even possible, my insert rad. changes, 431/432, and its the same discrepancy no matter what i put into the offset for the tool. heres another example, cutting a bore with G71 and G41 in the cycle. after i have a single line to clear material to allow a slip for bearing into the bore. the bore would cut to size, than on the single line (without C.C.) it cuts big. explanation of how one can use comp backwards would be appreciated. i use G42 on OD, G41 on ID.


Thanks
 
so out of curiosity,i went and put a G41 into my cycle on the OD turn, it allows it to run (thru graphics) but clearly show the tool path further into the part in comparison to G42. also should be noted i have another st30 i work on here that doesnt have these issues at all.
 
I meant you G41 and G42 mixed up. Like AirLake said, G41 on the OD will cut on the opposite side of your programmed path by the amount of radius in your tool comp. Looks like you are ok there.
I have no other ideas. Could you post the section of code?
 
Heres the code per request. the thing is it isnt just for this code, its any time i use a canned cycle with C.C.T606
G50 S2000
G97 S525 M03
G54 G00 X4.2 Z0.1 M08
G96 S420
G99
G71 P8 Q18 U-0.05 W0.005 D0.08 F0.013
N8 G41 G00 X5.2 Z0.1
G01 Z0. F0.008
X5.177
X5.117 Z-0.03
Z-1.615
X4.675
X4.625 Z-1.64
Z-2.1
X4.2
N18 G40 G00 X4.2
G53 G00 X-5. Z-10. M09
M05
M01


T1111
G50 S2500
G97 S750 M03
G54 G00 X4.2 Z0.1 M08
G96 S600
G70 P8 Q18
Z0.1
G00 X5.121 Z0.05
G01 Z-0.25 F0.005
G00 X5. Z0.1
G53 G00 X-5. Z-10. M09
M01


SO its rough/finish. the bore cuts to size but the 5.121 will cut at like 5.17. so while cutting in canned cycle with C.C. on it can hold the .0003 on the bore, but as soon as the canned cycle is done and C.C. is turned off it starts cutting at different dimensions. this is also messing with chamfers, since i cut the face without C.C. then try to cut chamfer in a canned cycle the z is off and usually my chamfer cuts in air, roughly .025 in front of what was z0. i just dont understand how a tool can come down at z0. in a program, cut and clean the face than be .025 off for the rest just with C.C. when i put a G41 in for an od turn it definitely cut further in (which is what i need) while in graphics. is there a setting that determines what G41/G42 do? or could it be that im not touching tools off with a probe, therefore not having the correct position in the offset for each tool?
 
Alright gentlemen (and ladies if present). it was the tip direction ni the offset for the tool.. i appreciate the help and input very much. will for sure be coming back any time i have an issue and randomly to see if i can help with any. thanks again everyone
 
The program above is a boring operation so you must use G41, not G42.

Also the boring bar tool geometry should be labeled "Tool Type #2" for a boring operation.

My Bad, Just noticed you solved the problem.
 








 
Back
Top