How to do Threading in Pro/NC

[shekar_ir]

Hello All,


Can Anbody pls let me know how to do the Threading Operation in Pro/Nc


The problem actually is after defining my Machine,Workcell and Operation.When i define a new NC sequence for Threading When i try to pick the tool for threading it says "This is not a valid tool" Pls let me where am i wrong


Thanks


Chandra

 

[chf65]

Make a THREAD_MILL tool type. It only works with THREAD_MILL tools.


Charles

 

[peterbrown77]

Unless, of course, she is trying to tap a hole in which case she needs to do a holemaking sequence, not a thread sequence.





Regards

 

[paulstern]

Another problem you may run into if you are using a thread mill that is not single point is that the automatic sequence may make too many passes. You can control this with number of teeth parameter in the tool dialog. Rather than this describing the number of flutes it describes the number of threads that can be cut with one pass of the tool.

 

[appinmi]

I use a "trajectory" milling sequence to do my thread milling. It requires 2 "automatic cuts"


The first cut will be the lead-in only. set the parameter "axis shift" to the top of the thread.


The second will be the lead-out only. If you need to, set "axis shift" to the bottom of the thread. Set clearance to the distance from "top of thread" to "bottom of thread". Set "lead radius" to the radius you want the cutter to travel. Set tangent and normal approach to zero. Set "entry angle" to ("clearance/pitch). Then add a "helical lead-in" to the second cut, and click "done cut"


Delete the "retract" and second "auto plunge", and your done. If you have done it correctly, the end of the dirst path and the beginning of the second path will be the same point, therefore you will see no "extra" goto in the cl file.


With a little imagination, you can even add "cutter comp" with "a CL command".