Using Oak/CNC12 Lathe with HSMWorks CAM

[simmonds]

I have gotten the retrofit of my Hardinge/Accuslide gang-tool lathe mostly finished (see pictures). Thanks for all the help provided by the kind and knowledgeable folks on this forum. Now I am now starting to think about how to best generate my G-code.

I have used my SolidWorks/HSMWorks CAM program extensively to run my Haas TM-1 mill and would like to use it with the Centroid system installed on this lathe. Although the Centroid interactive programming is much more intuitive than Haas, I have gotten rather spoiled by having a CAM program that is so feature-rich and automatically updates cutter paths when I modify my SolidWorks part file.

There do not appear to be any Centroid-specific posts available for the lathe, but from what I have read online, it is quite similar to a Fanuc. Should I start with that? Are there any well-known incompatibilities that I need to be aware of.

Since the lathe is configured with gang-tooling, it does not need automatic-tool-changer commands. But it also does not need to pause while I manually change a tool. What is the best way to tell the Centroid to switch to a new tool/offset without having it wait for manual intervention?

Finally, for tools that are mounted behind the work (e.g. a parting tool) what is the best strategy for getting the spindle direction and approach direction reversed. If the CAM program and the Centroid both try to implement the reversals, it will not be good.

As you can see from my report file, I am using the "stock" lathe PLC program and have not yet set up any tool offset library.

[cncsnw]

Since the lathe is configured with gang-tooling, it does not need automatic-tool-changer commands. But it also does not need to pause while I manually change a tool. What is the best way to tell the Centroid to switch to a new tool/offset without having it wait for manual intervention?

Create a "cnctch.mac" file which contains nothing but a comment.

Finally, for tools that are mounted behind the work (e.g. a parting tool) what is the best strategy for getting the spindle direction and approach direction reversed. If the CAM program and the Centroid both try to implement the reversals, it will not be good.

Except for X and Z offsets, nose radius and nose vector, all the information in the Centroid tool library is just for the benefit of the Centroid Intercon software. If you are running CNC codes from any other source (e.g. your CAD/CAM software), then the control just does what the G codes tell it to do (e.g. run the spindle forward if M3; run the spindle reverse if M4; go to positive or negative X coordinates as specified in the G codes).

Tools which cut on the negative side of the spindle will need to be programmed with negative X coordinates.

[simmonds]

Thanks for the information.

Selecting spindle direction is part of the CAM's tool description. I will just need to convince it to reflect the X coordinates about zero for that tool.

It is very convenient that the too change commands are located in a macro. Did not know that.

[DICKEYBIRD]

Bee-yoo-ti-ful lathe sir; kudos! I'm green with envy.

[simmonds]

I found an Autodesk/Fusion360 FANUC Lathe post that "FRANCO" modified to work with the Centroid Lathe control. He has a video and and a dropbox link to that post that can be found here:


Conveniently, all Autdesk CAM programs (HSMWorks, Fusion360) use the same post processors.

He fixed several issues with the standard FANUC post, as he clearly describes in his video. These include the formatting of comments, unsupported plane (G17-G19) commands, and unsupported drill cycles (which he expanded to inline G-code).

But his modifications were done to a post dated 2017-09-14 which did not support Front/Rear mounted tools, as I have with my gang-tool lathe. So I "ported" his fixes over to a newer (2018-11-02) FANUC Lathe post that does support this feature. And I added a couple of my own tweaks.

I changed the dwell-time units from milliseconds to seconds, as Centroid expects:
G4 P0.1 means 0.1 seconds.

I also changed the meaning of the Turret numbers 101, 102, 103 and 104 so that 101 and 103 (FRONT mounted tool) have the tool start from a positive X value and move in the negative X direction. It is the opposite for 102 and 104 (REAR) tools. See the Property window Tool Tips. Perhaps I am missing something, but this X-axis orientation made more sense to me. In any event, it is easy to change this back (near line 730 in the .cps file)

Note that spindle direction must be specified in the tool description and is not affected by using FRONT or REAR mounting.

Just as FRANCO did, I have only commented out (not removed) lines that were modified. To facilitate searching, his name and my initials (MBS) are at the end of all lines that he or I have modified or added.

I had to change the extension from .cps to .txt in order to upload the file.

[tblough]

So nice to see another well done Hardinge conversion!