Showing results for 
Search instead for 
Did you mean: 

G70 ,G71, G72, G73, G75, G76 Turning Cycles using NX CAM


There was different Turning cycles available in Fanuc series oi-tf. But i don't how to Create it with the help of NX CAM. If anyone knows about it pls share.


Re: G70 ,G71, G72, G73, G75, G76 Turning Cycles using NX CAM

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom

first, you have to turn the cycle output  in nx turning operation.

second - try to create PP - lathe, fanuc controler.

it has it implemented g70,71,72 i think...

#♫ PB, 5ax, itnc, nx, vericut ♫ #

Re: G70 ,G71, G72, G73, G75, G76 Turning Cycles using NX CAM

Gears Esteemed Contributor Gears Esteemed Contributor
Gears Esteemed Contributor

For certain operations, this is relatively easy (OD/ID/Face rough)

For others, it is "doable" but harder (involving a lot of TCL code in PB) (threading - G76 / G92, G276 on Mazak, etc.)

For "finish" passes, (IMHO) it's not worth it - just cut the finish pass in NX.

I don't think grooving can be done, as the required info is not there (note if you do this, the motion shown in NX may NOT match the actual motion on the machine) (if you REALLY want to do grooving, you may have to "fake" the data in NX to get the profile of the groove)


I only have experience with Post Builder, Post Configurator may be somewhat different


OD/ID/Face rough

1) In operation in NX part, you must set the "Motion Output" (Typically found in the  "Machine Control" block) to "Machine Cycle"

2) Create your PB post using one of the "specific" "Library" controls (in PB 10.0.1, Fanuc or Siemens or whatever) - so when you go to "Program & Tool Path" -> "Progam" tab -> "Canned cycles", (you may need to scroll down) you see a "Lathe Roughing" cycle under the "Bore" cycle.



You have to "intercept" all the threading motion/events, calculate your values, then output the macro.

You may be able to get some example code from GTAC (that's what I started with).

Remember, NX outputs (at least) *4* events *per thread pass* (the "engage" move, the "cut" move, the "retract" move, and the "return to starting point" move) The engage may have a couple moves (depending on infeed).  So you need to process a bunch of tcl variables to see if you can even output a cycle. 

This is "non-trivial", but can be done.

A partial list of variables:



mom_tool_right_angle, mom_tool_left_angle


mom_lathe_thread_lead_i, mom_lathe_thread_lead_k

mom_total_depth_finish_passes_number_of_passes  ;# an array





mom_turn_thread_root_line   ;# an array 

mom_turn_thread_crest_line  ;# an array




Hope this helps...Ken

Ken Akerboom Sr CAx Systems Engr, Moog, Inc.
Production: NX10.0.3.5 MP16/TC11.2
I'd rather be e-steamed than e-diseaseled

Learn online

Solution Information