G92 threading getting strange code

[Anonymous]

Have a look at code here. I am trying to do a simple 1/2-20 external thread with a G92 cycle. It keeps posting code with G1 moves and a feedrate of zero before and after threading. 

[engineguy]

@Anonymous 

What Post Processor are you using ??

Here is the code I get using the Standard Fanuc Turning Post Processor:-

(THREAD1)
N14 T0101
N15 G54
N16 M8
N17 G99
N18 G97 S500 M3
N19 G0 X1.3 Z0.1969
N20 G0 Z0.01
N21 G92 X0.48 Z-0.2444 F0.05
N22 X0.464
N23 X0.448
N24 X0.432
N25 X0.416
N26 G0 X1.3 Z0.1969

N27 M9
N28 G28 U0.
N29 G28 W0.
N30 M30
%

Looks fine to me, PP used attached.

Stay Safe

Regards

Rob

[Anonymous]

@engineguy 

 I used that post you attached and got the same results. Maybe its something with the project I set wrong?

[engineguy]

@Anonymous 

It is your settings in the NC Program, I changed it and it seems to work OK now, I have attached the modified file for you to test.

Make sure that you have the PP I/we used in your "Personal Post Library" as that is the path I set in the NC Program, see image, or re-set it to where you have that Fanuc PP located at your end 🙂 🙂

(THREAD1)
N116 M1
N117 T0707
N118 G54
N119 M8
N120 G99
N121 G97 S500 M3
N122 G0 X0.836 Z0.1969
N123 G0 Z0.232
N124 G92 X0.4872 Z-0.202 F0.05
N125 X0.4784
N126 X0.4696
N127 X0.4608
N128 X0.452
N129 G0 X0.836 Z0.1969
N130 M9
N131 G28 U0.
N132 G28 W0.

Stay Safe

Regards

Rob

[Anonymous]

@engineguy  Thank you for helping....I would like to get this fixed.  I have loaded the part file you sent and used the post we used before and still get zero feedrate moves. Tried a couple different posts and get the same bad moves. 

[zwelsh91 · Accepted solution]

Are you using Fusion 360 under a personal entitlement? I notice the program header is notifying you of some variables that are different from the Personal License to a Commercial Subscription. I would suspect that you are running into problems based on that over the Post Processor. They have removed the availability to use "G0" Rapid movements for Personal License Users. Have you defined a high feed rate for your machine?

[Anonymous]

Ahh, didn't even consider that.... We run HSMworks at work with Fusion 360 entitlement, tomorrow I will try to install the full version there and retest. Will report back.

Thank you.

[engineguy]

@Anonymous 

What Zac@zwelsh91 is saying that in the Header of your code it is saying that you have no Rapid moves, so do what @zwelsh91  suggests and set a high feedrate instead of Rapids.

Unfortunately the only proper fix is to pay for the software now 😞 😞 😞

Stay Safe

Regards

Rob

[Anonymous]

Are you using Fusion 360 under a personal entitlement? 

[Anonymous]

Are you using Fusion 360 under a personal entitlement? 

192.168.100.1 192.168.1.1 jpg to pdf

[Anonymous]

Yes, I am. I assume that is the issue now. Thanks