Announcements
Attention for Customers without Multi-Factor Authentication or Single Sign-On - OTP Verification rolls out April 2025. Read all about it here.

Lathe Thread retract to clearance plane is slow

finchmAQDUT
Explorer

Lathe Thread retract to clearance plane is slow

finchmAQDUT
Explorer
Explorer

 

thread pic 2.jpgthread pic.jpg

 

I am cutting 8 tpi threads 1/2" long on 1" diameter bar.  I believe that I have all the parameters that I am able to configure set correctly.  I am using the 'Generic FANUC Turning" post processor.

 

The G code that is generated has an incredibly slow retract to the clearance plane.  A snippet of the g code is below:

 

N18 G97 S500 M3
N19 G0 X1.4 Z1.
N20 G1 X0.986 F10.
N21 G32 Z-0.5 F0.125
N22 X1.14 F0.125
N23 G0 X1.4
N24 Z1.
N25 G1 X0.9802 F10.
N26 G32 Z-0.5 F0.125
N27 X1.14 F0.125
N28 G0 X1.4
N29 Z1.

 

The red highlighted retracts are occurring at a feedrate of .125.  I would be happy with the leadout feedrate of 10 in/min or the rapid feedrate.  How do I adjust the retract speed?

 

0 Likes
Reply
666 Views
6 Replies
Replies (6)

LibertyMachine
Mentor
Mentor

Is this a modified post processor? Using default settings and a generic Fanuc post, I am not getting what you are:

N18 G97 S500 M3
N19 G0 X1.3811 Z0.1969
N20 G0 Z0.0333
N21 G1 X0.5838 F10.
N22 G32 Z-0.7133 F0.07874
N23 X0.6747 Z-0.7587 F0.07874
N24 G0 X1.3811
N25 Z0.0333
N26 G1 X0.5692 F10.
N27 G32 Z-0.706 F0.07874
N28 X0.6747 Z-0.7587 F0.07874
N29 G0 X1.3811
N30 Z0.0333

 

The short retract move from X.5838 to X .6747 is at a slower feedrate, but then kicks up to a rapid.

 

What do you have for Clearances (on the Clearances tab)?

 

Did you modify these choices:

screenshot_33.png

 

If neither of those are the case, could you share your part so we could see the choices made and determine how they are producing what you are seeing? File > Export > Save to local folder. Attach the .f3d in your reply


Seth Madore
Owner, Liberty Machine, Inc.
Good. Fast. Cheap. Pick two.
1 Like

finchmAQDUT
Explorer
Explorer

I believe clearance was .20 inches, and that somehow became .14 in post. I didn't modify any of the post settings. 

 

Your post is very similar to mine.  you have the same slow retract at the threading rate, but in your example it looks like you are tapering off the threads.

 

.lines n23 and n28 taper upwards from the thread depth from z -.7133 to -.7587. I want my threads to just stop as I already have a relief cut at the end. 

0 Likes

finchmAQDUT
Explorer
Explorer

Here is the file.

0 Likes

Steinwerks
Mentor
Mentor

It's definitely feeding out, you can see it if you use View Toolpath (expand the toolpath with the triangle next to it, right-click the bottom icon with the KB size of the path, and select View Toolpath):

 

Feed Out.JPG

 

I'd definitely classify this as "something that needs work" as it has the potential to scrap parts IMO.

 

@paul.clauss can you provide some feedback on this one?

Neal Stein

New to Fusion 360 CAM? Click here for an introduction to 2D Milling, here for 2D Turning.

Find me on:
Instagram and YouTube
0 Likes

paul.clauss
Alumni
Alumni

Hi @Steinwerks@finchmAQDUT

 

Thanks for bringing this one to my attention! I will show this to some other members of the team and get back to you as soon as possible - which may be early next week.

 

 

I was unable to find a setting or anything that may have been missed in the setup and received the slow retract rate as well as the inconsistent retract distance. We will be looking into this issue!

 

Please let me know if you have any questions!

Paul Clauss

Product Support Specialist




0 Likes

cj.abraham
Alumni
Alumni

This may be an issue in the post that is picking up the pitch of the thread for a "general" feedrate. I'm looking into it more.

 

Edit: It's a software issue. update to come.

0 Likes