I am chamfer milling the hole shown in the picture. The path is exactly what I want the machine to do, but NX is outputting it as 7 separate arcs (9 counting engage and retract). Personally I wouldn't mind it if the machine made a chamfer, but the operators hate seeing something like this. Is there anyway in NX to combine these moves into 1 arc like it should be? Also if possible is there anyway I can control the position on where it starts? I made the operation using z-level-profile.
PAINT/PATH PAINT/SPEED,10 PAINT/COLOR,186 FROM/2.5000,0.0000,-5.0000,1.0000000,0.0000000,0.0
000000 LOAD/TOOL,5,ADJUST,5 RAPID GOTO/0.7675,-0.3000,0.8405 PAINT/COLOR,211 RAPID GOTO/0.3165,-0.3000,0.8405 PAINT/COLOR,6 FEDRAT/IPM,18.0000 GOTO/0.2165,-0.3000,0.8405 CIRCLE/0.2165,-0.2282,0.6010,-1.0000000,0.0000000, 0.0000000,0.2500,0.0020,0.5000,0.5000,0.0000 GOTO/0.2165,-0.4677,0.5292 PAINT/COLOR,31 GOTO/0.2165,-0.4613,0.5080 CIRCLE/0.2165,0.0000,0.6687,-1.0000000,0.0000000,0 .0000000,0.4885,0.0020,0.5000,0.5000,0.0000 GOTO/0.2165,0.0000,0.1802 CIRCLE/0.2165,0.0000,0.6687,-1.0000000,0.0000000,0 .0000000,0.4885,0.0020,0.5000,0.5000,0.0000 GOTO/0.2165,0.4613,0.5080 CIRCLE/0.2165,-0.0014,0.6685,-1.0000000,0.0000000, 0.0000000,0.4897,0.0020,0.5000,0.5000,0.0000 GOTO/0.2165,0.4613,0.8292 CIRCLE/0.2165,0.0000,0.6691,-1.0000000,0.0000000,0 .0000000,0.4883,0.0020,0.5000,0.5000,0.0000 GOTO/0.2165,0.0000,1.1573 CIRCLE/0.2165,0.0000,0.6691,-1.0000000,0.0000000,0 .0000000,0.4883,0.0020,0.5000,0.5000,0.0000 GOTO/0.2165,-0.4613,0.8292 CIRCLE/0.2165,0.0028,0.6682,-1.0000000,0.0000000,0 .0000000,0.4912,0.0020,0.5000,0.5000,0.0000 GOTO/0.2165,-0.4884,0.6744 CIRCLE/0.2165,0.0016,0.6682,-1.0000000,0.0000000,0 .0000000,0.4900,0.0020,0.5000,0.5000,0.0000 GOTO/0.2165,-0.4740,0.5504 GOTO/0.2165,-0.4735,0.5485 GOTO/0.2165,-0.4677,0.5292 PAINT/COLOR,1 CIRCLE/0.2165,-0.2282,0.6010,-1.0000000,0.0000000, 0.0000000,0.2500,0.0020,0.5000,0.5000,0.0000 GOTO/0.2165,-0.1564,0.3615 GOTO/0.3165,-0.1564,0.3615 PAINT/COLOR,211 RAPID GOTO/0.7675,-0.1564,0.3615 PAINT/SPEED,10 PAINT/TOOL,NOMORE END-OF-PATH
Solved! Go to Solution.
The listing will always show the arcs in 120 degree segments, but the post should output in either full arcs or quadrants.
What is coming out or the post?
BTW, what operation type is this? I notice the arc center is moving around a bit.
X.633 G01 X.433 Y.2402 Z.4165 G03 Y.4878 Z.6689 J-.0024 K.25 G01 Y.4875 Z.6977 Y.4832 Z.7397 G03 Y-.4832 J-.4832 K-.0714 G01 Y-.4846 Z.7289 Y-.4884 Z.6723 Y-.4885 Z.6664 Y-.4841 Z.604 Y-.4834 Z.5981 G03 Y-.4059 Z.3967 J.4888 K.0724 G01 Y-.397 Z.3839 G03 Y.4834 Z.5981 J.3969 K.2848 G01 Y.488 Z.6479 Y.4878 Z.6689 G03 Y.2354 Z.9165 J-.25 K-.0024 G01 Y.1641 Z.8414 X.633
This is what is coming out of the post. I just noticed that the extend surface option is causing the issue with the post. I got rid of it and it did post out 3 arcs like it was suppose to. The reason I need the surface extended is because it is a chamfer tool and the tip isn't a sharp point like the computer. It needs to cut further up the tool. Is there a way I can cut like this and get a 3 arcs?
Is there a reason for using Z-Level profile? Could it just be a planar profile operation? I just pick the diameter of the chamfer being cut, set my floor past the chamfer depth and generate.Maybe the surface isn't planar, I can't tell.
G00 G90 G54 X.1125 Y-.1875 G43 H01 Z.5 M08 Z.025 G01 Z-.075 F10. G03 X.3 Y0.0 I0.0 J.1875 G03 I-.3 J0.0 G03 X.1125 Y.1875 I-.1875 J0.0 G01 Z.025 G00 Z.5
would you mind giving me a copy of that file, I tried planar profile, but I can't get it to cut below the plane of the curve. Also the tool only seems to want to be tangant to the shank of the tool at the center point of the tool. Is there an option to planar milling I am not seeing?