Community
Fusion Manufacture
Talk shop with the Fusion (formerly Fusion 360) Manufacture Community. Share tool strategies, tips, get advice and solve problems together with the best minds in the industry.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

Lathe Post thread milling feed rate issue.

15 REPLIES 15
Reply
Message 1 of 16
ronBZV6V
428 Views, 15 Replies

Lathe Post thread milling feed rate issue.

I have noticed something unusual while running some milling toolpath on my Smart Machine Tool NL2000M CNC Lathe.

(Live tooling no Y axis). While contouring the feed rate is outputting normally but while trying to run any inside toolpath like boring with a milling tool and thread milling the feed rate while running in incredibly slow. I'm still learning Lathe G-code so I'm not sure what to change either in the post itself or something in Fusion 360 I can change to correct this issue. I am attaching both the posted code and the Fusion file for reference. Outside milling is normal "inside" Milling runs way too slow. (boring/ threadmilling ops) 

 

Note: this file is just an example file to show what I mean not and actual part. I'm just trying to figure out how correct the issue for future parts. 

15 REPLIES 15
Message 2 of 16
BrandonTBFBF
in reply to: ronBZV6V

Which post are you using?

 

The feedrates that are being output are 4800. If this is Inches per Minute, that might have something to do with it.

Message 3 of 16
ronBZV6V
in reply to: BrandonTBFBF

It's a generic Samsung post from fusions generic list modified to remove Y-axis. I can't even see where it's getting the F4800. from. I don't know where to start with this. 

Message 4 of 16
BrandonTBFBF
in reply to: ronBZV6V

What control is on the machine? Does it have Polar Interpolation (G12.1)?

 

The 4800 is the maximum degrees per minute feed in the Multi-axis feedrate logic.

Message 5 of 16
ronBZV6V
in reply to: BrandonTBFBF

Its a Fanuc Oi-TF plus.

 

It shows a G12.1 in my machines training manual so I'm assuming it works. I'm not sure I've ever seen it used on the machine yet.  

Message 6 of 16
BrandonTBFBF
in reply to: ronBZV6V

Try these two version out. 

 

The first just has the Maximum DPM feed bumped up to 99999. If you back calculate the feed at .023" radius and 4800IPM you get an effective feed of 1.92IPM. This might be what you're seeing.

 

The Polar version has Polar Interpolation enabled.

Message 7 of 16
ronBZV6V
in reply to: BrandonTBFBF

Thank you I will give these a try (carefully of course) and report back my findings. 

Message 8 of 16
ronBZV6V
in reply to: BrandonTBFBF

Neither of these work. The polar one gives me an "illegal plane selection error" on the machine and the other runs about the same speed as before. 

Message 9 of 16
BrandonTBFBF
in reply to: ronBZV6V

I see the plane problem. It defaults to G18. I've changed it to G17.

Message 10 of 16
ronBZV6V
in reply to: BrandonTBFBF

Thank you I'll try this as soon as I get the machine off of the job its on now. 

Message 11 of 16
rdwilkes
in reply to: ronBZV6V

I'm running the same machine, wondering about your test results.

Message 12 of 16
ronBZV6V
in reply to: BrandonTBFBF

This also gives me an illegal plane selection error. As soon as it see the G17.  Sorry for the inconvenience. I just got back to running this job again. 

 

Thank you so much for your help,

Message 13 of 16
ronBZV6V
in reply to: BrandonTBFBF

Any suggestions as to what I should do next?

Message 14 of 16
BrandonTBFBF
in reply to: ronBZV6V

I'm not sure why G12.1 isn't working.

 

Have you tried thread milling a large diameter with the non-polar post? I'd be curious to know if the machine looks like it's running the correct speed when not near X0.0

Message 15 of 16
ronBZV6V
in reply to: BrandonTBFBF

I will check on this as soon as possible. 

Message 16 of 16
ronBZV6V
in reply to: BrandonTBFBF

I finally have an answer as to what is the problem. Come to find out my machine doesn't have the option turned on for helical interpolation. Apparently its an option they can activate for about $1500 nothing more than turning on the option in the controller.  Something only Fanuc employees can do. 

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums