Cancel
Showing results for 
Search instead for 
Did you mean: 

OUTPUT THREAD CYCLE IN NX?

Pioneer
Pioneer

THERE IS WAY TO OUTPUT THREAD CYCLE IN NX? i DID NOT FIND THIS OPTION.

-----------------------------------------
UG3.0
UG6.0
NX10.0.35
NX11.0.1
UG_NX is my favorite !!!!!!
5 REPLIES

Re: OUTPUT THREAD CYCLE IN NX?

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom

Thread made with tap? or thread made with thread-mill? or thread made on a lathe?

 

For tapping - yes, there is OOTB cycle.

 

For thread milling and thread turning cycle output, you will need to make significant customizations in postprocessor - if you want to use regular CAM operations.


For thread milling it is also possible to create something like "user defined cycle".

Marek Pawlus, NCmatic

Production: NX 12.0.1
Development: C#, Tcl/Tk, CSE

Re: OUTPUT THREAD CYCLE IN NX?

Gears Phenom Gears Phenom
Gears Phenom

I was into this topic too. (if you are talking about milling)

 

- Drill text, cycle option

- Creating user defined cycle - still drilling cycle, axial movement of the tool

 

In both cases you wont see milling in simulation and you have to create ude parameterers for filling cycle parameters. But Some api can collect feature parameters.

 

In general machine cycles - thread milling , hole milling  - has different tool paths as you can set in nx.

I am not very familiar with making thread and hole milling like cycle output.

There is lots of work (for perfect match between machine cycle and nx tool paths) on it and no output like drill cycles - cycle postions, cycle plane change, etc.

 

Helical output can shorten the nc file - this is enough for me.

 

---------------------------------------------
#♫ PB, 5ax, itnc, nx, vericut ♫ #

Re: OUTPUT THREAD CYCLE IN NX?

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom

I'm also not a fan of outputting canned cycle from regular CAM tool path. Like for Rough Turning or Hole Milling or Thread Milling.

With CAM tool path we can set so many options which are not handled by canned cycles...

Sooner or later, if user don't understand how this canned cycle works, he will start complaining that:

- "I set this parameter in CAM operation, it is simulated well in NX Verify, but machine did it differently!"
- of course it did, because canned cycle is mostly much less complex...

Marek Pawlus, NCmatic

Production: NX 12.0.1
Development: C#, Tcl/Tk, CSE

Re: OUTPUT THREAD CYCLE IN NX?

Pioneer
Pioneer

As thread cycle on the lathe.

 

I output CL data like this.

 

Cycle / Thread,xxx.............

Goto / XXX.......

;;;

Goto / XXX.......

;;;

Goto / XXX.......

;;;

 

Am I not sure this is correct output?

 

 

-----------------------------------------
UG3.0
UG6.0
NX10.0.35
NX11.0.1
UG_NX is my favorite !!!!!!

Re: OUTPUT THREAD CYCLE IN NX?

Gears Esteemed Contributor Gears Esteemed Contributor
Gears Esteemed Contributor

how the CLS "CYCLE/THREAD" is handled depends on the post.

 

OOTB UGPost posts will output (for each thread pass)

- "engage" move to proper diameter (typically G0 or G1)

- "cut" move - thread pass (typically G3x - e.g. G32 or G33 or G34)

- "retract" move away from the parts surface (typically G1 or G0)

- "return" move to start point (typically G0)

 

Most of the above can be customized (e.g. engage and/or retract could be G3x command, you can add an additional engage direction, etc.)

 

But all this can be customized in UGPost to

- G9x cycle (G92 or G96 or ...) - one line to set feed & Z dimension, followed by "X" moves - one per diameter)

- full thread cycle (G76 or G276 or ...) - one or 2 lines specifies the whole thread.

 

But, as others point out, you lose a lot of NX's ability to get "exactly" what you want specified in NX & see it on the machine. 

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