We have a problem abaout Cavitiymill_Adaptive milling. When we use at adaptive milling operations, first tool path always have so many cut steep points. But normally it doesnt need many cut step. Because its only one axis moving. (like going x-5. to x-10. ) Our machines have high speed reading qualitication. Because of the cut step points machine always changing F speed. In other strategies we dont have same problem. (For exapmle: fallow_periphery) For finish operastions (like counter area) we can change cut step. But in cavity mill its not possible. I send the operation photo and post file. Any can help us please?
We use NX 22.214.171.124.
Hey @Fwerkstatt ,
welcome to the NX Manufacturing Forum
I can see that you are working with the Preview version of Adaptive Milling, since you are on NX11. Adaptive Milling was first released in NX12. We added a lot of enhancements to Adaptive Milling, including Arc Output for the post run.
I wouldn't compare the traditional approach in Cavity Mill with Adaptive Milling, since they are working completely different.
Additionally, I would suggest to add the HSC Cycle with the Roughing option on your machine controller. At Sinumerik it is Cycle832 and on Heidenhain it is Cycle32. Not sure about Fanuc and Mazak. As the tolerance just set a bit less then your stock. Typically between 0.05mm and 0.15mm is being used at a part stock of 0.2mm.
Would it be possible to try in the newer official versions?
Hey Thank you for you recommendations. i usually doing cavity operations with part stock 0.15 and intool´-outtool tolerances 0.03 . i tried your solution and changed with 0.07. Now its a little better but still there are so many cut step points. I have never used Cyle832. We have sinumerik_840d control units. Can you send me example post which has cycle832 code please. We have post builder license i can add cycle832. But we dont have NX12 license. So i cant try new version adaptive milling .
Thank you for your help.
We have heidenhain control unit
CYCLE 32 parameter
CYCL DEF 32.0 TOLERANCE
CYCL DEF 32.1 T0.1
CYCL DEF 32.2 HSC-MODE:0
We use T value 0.1 for roughing and program stock should be greater than T tolerance.
HSC mode value represents operation type.0 value is for finishing, 1 value is aggressive roughing.
I dont know post tolerances for sinumerik control,you can look for sinumerik control manuel to learn.
If you have a part stock of 0.2 mm, then you can defintely make 0.15 mm tolerance
CYCLE832(0.15,3,1); (Roughing with Tolerance 0.15)
Assuming you do have an 840D controller.
@Fwerkstatt Again, be careful, you are using Pre Release Software with Adaptive Milling in NX11! It wasn't released in NX11.