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.
Showing results for 
Show  only  | Search instead for 
Did you mean: 

Lathe CAM - axial offset when using rear threading tools.

Message 1 of 6
276 Views, 5 Replies

Lathe CAM - axial offset when using rear threading tools.

My CNC lathe has a rear mounted turret ATC and the spindle rotates clockwise when viewed from the tailstock. This means that normally I have to use "left hand" tools" for turning towards the headstock. In the case of threading inserts, they are left hand so that the threading point is towards the headstock although these are usually sold as "internal" if using the 3 point style.


If I am threading close to the tailstock, I need to use a RH toolholder, which is similar to using a LH toolholder in a conventional lathe. However, when I select a RH toolholder, the toolpath becomes offset axially by something like 12mm (most of the threaded length).


No confinement limits.png


The only way I can resolve the issue is to set the confinement limits to -11.5 and +14mm. Clearly something is wrong here!


Confinement limits.png


In general, the tool library is very basic and clunky, like it hasn't been fully developed and tested yet. When you combine that with the lack of error messages, setting up and getting toolpaths to run can be a matter of significant trial and error with no idea how long it will take to get a result.


For icing on the cake, the preview shows a LH thread even though the spindle rotation and feed direction are correct for a RH thread as intended.


Toolpath 16mm x 20tpi.png


LH thread shown in sim.png

Message 2 of 6
in reply to: Muzzerboy

@akash.kamoolkar - did you see this? Could you reply / comment and possibly add it to your bugs list / action tracker?


Many thanks

Message 3 of 6
in reply to: Muzzerboy



Message 4 of 6
in reply to: Muzzerboy

This isn't so much a question for Akash as it is a question for the tool library folks.

The reason that it's offsetting the toolpath the amount it is is because of where the toolpath pulls the "tip" of the tool from. In the case of your RH tool mounted as you have it, it (the toolpath) has to take into account the tool_overallLength parameter. We can use that information to make an expression where the Backside Offset is -tool_overallLength and the Front Side Offset is (threadPitch*5)-tool_overallLength. Result:



I would then save this toolpath as a Template and then it becomes a simple matter of calling that up instead.



And yes, there is certainly internal discussions about the CW/CCW and how a tool is displayed in the library. 


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 5 of 6
in reply to: Muzzerboy

@Muzzerboy I've created a ticket for this. We will revisit this issue once the tool library team has finished its work of decoupling the spindle direction from tool orientation (as Seth mentioned).



Akash Kamoolkar
Software Development Manager
Message 6 of 6
in reply to: akash.kamoolkar

Many thanks for the replies, Seth and Akash! I assumed Akash was the primary contact as the lathe CAM coordinator here.


Sorry I didn't see this and reply earlier, as I've been away on business and leave. Glad it makes sense and you have raised a ticket so it gets added to your issue tracker.


I appreciate some of this front / back / left / right / CW / CCW stuff is a logical nightmare. It also ties in with the rather cryptic and almost-hidden "Turret 102" etc settings in the tool library, which caused me and others some head scratching. 


On a related note, there doesn't seem to be any way to select "LH" tooling for use on a rear turret with CW spindle, particularly the insert and how it is shown in the toolholder. For this job I was able to use a "conventional" ie RH tool , as the threaded portion was not up against a shoulder at the headstock end. But for most threading jobs I'd have to use a LH tool and what is often sold as an internal threading insert. Currently there doesn't seem to be any way to set this up in the tool library and there's no tool / insert editor as there is in the milling tool library.


BTW, thanks for reminding me of the expression editor! I will make use of that to work my around some of these issues if they arise.

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

Post to forums  

Autodesk Design & Make Report