NX Getting Started with the New Motion Output -> Machine Cycle in Thread and Hole Milling
2021-10-06T23:27:36Z
NX for Manufacturing
Summary
Details
In NX1899 a new option named Motion Output was added to the Thread and Hole Milling menus. The two available settings for this new option are Single Moves and Machine Cycle. What do these new options do and how would Post Builder be setup to use them?
G00 G90 X50. Y50.
G43 Z75. H14 S500 M03
Z25.88
G01 X54.782 Y48.72 F250. M08
G03 X56.45 Y50. Z26. I.343 J1.28 K.065
X56.45 Y50. Z28. I-6.45 J0.0 K.318
X54.782 Y51.28 Z28.12 I-1.326 J0.0 K.065
G01 X50. Y50.
G00 Z33.88
G01 X54.782 Y48.72
G03 X56.45 Y50. Z34. I.343 J1.28 K.065
X56.45 Y50. Z36. I-6.45 J0.0 K.318
X54.782 Y51.28 Z36.12 I-1.326 J0.0 K.065
G01 X50. Y50.
G00 Z41.88
G01 X54.782 Y48.72
G03 X56.45 Y50. Z42. I.343 J1.28 K.065
X56.45 Y50. Z44. I-6.45 J0.0 K.318
X56.45 Y50. Z46. I-6.45 J0.0 K.318
X43.55 Y50. Z47. I-6.45 J0.0 K.318
X45.218 Y48.72 Z47.12 I1.326 J0.0 K.065
G01 X50. Y50.
G00 Z75.
If this same hole would be milled with the Machine Cycle switch selected than the code might look similar to that seen below. Notice that instead of helical motion a cycle command is output.
G00 G90 X50. Y50.
G43 Z75. H14 S500 M03
Z50.
G65 P9012 X50. Y50. Z26. F250. R50. P2.0 Q10
G00 Z75.
To get this output from Post Builder would require that a User Defined Cycle be created.
When creating the User Defined Cycle it is important that the Cycle Name be mill_hole_thread for the thread data to be read.
The name of the hole mill User Defined Cycle would need to be mill_hole.
After the custom cycle is created the MOM variables from the thread or hole operation can be read and then output as G-code commands.
OS: n/a
OS Version: n/a
Product: NX
Application: CAM
Version: V1903
Function: HOLE_BOSS_MILL
Ref: 002-8017325
Solution
In previous versions of NX, a thread or hole milling operation would have been cut using helical G-code motion. This output would look something like the code seen below. This is the behavior that is now seen if selecting the Single Moves switch on this new menu. The Single Moves setting, therefore, is what would be used to get output as seen in older versions of NX.G00 G90 X50. Y50.
G43 Z75. H14 S500 M03
Z25.88
G01 X54.782 Y48.72 F250. M08
G03 X56.45 Y50. Z26. I.343 J1.28 K.065
X56.45 Y50. Z28. I-6.45 J0.0 K.318
X54.782 Y51.28 Z28.12 I-1.326 J0.0 K.065
G01 X50. Y50.
G00 Z33.88
G01 X54.782 Y48.72
G03 X56.45 Y50. Z34. I.343 J1.28 K.065
X56.45 Y50. Z36. I-6.45 J0.0 K.318
X54.782 Y51.28 Z36.12 I-1.326 J0.0 K.065
G01 X50. Y50.
G00 Z41.88
G01 X54.782 Y48.72
G03 X56.45 Y50. Z42. I.343 J1.28 K.065
X56.45 Y50. Z44. I-6.45 J0.0 K.318
X56.45 Y50. Z46. I-6.45 J0.0 K.318
X43.55 Y50. Z47. I-6.45 J0.0 K.318
X45.218 Y48.72 Z47.12 I1.326 J0.0 K.065
G01 X50. Y50.
G00 Z75.
If this same hole would be milled with the Machine Cycle switch selected than the code might look similar to that seen below. Notice that instead of helical motion a cycle command is output.
G00 G90 X50. Y50.
G43 Z75. H14 S500 M03
Z50.
G65 P9012 X50. Y50. Z26. F250. R50. P2.0 Q10
G00 Z75.
To get this output from Post Builder would require that a User Defined Cycle be created.
When creating the User Defined Cycle it is important that the Cycle Name be mill_hole_thread for the thread data to be read.
The name of the hole mill User Defined Cycle would need to be mill_hole.
After the custom cycle is created the MOM variables from the thread or hole operation can be read and then output as G-code commands.
Hardware/Software Configuration
Platform: allOS: n/a
OS Version: n/a
Product: NX
Application: CAM
Version: V1903
Function: HOLE_BOSS_MILL
Ref: 002-8017325