Tool path will not generate with tool orientation set to top approach.

[BillGEGHV]

Hi all,

I am new to CNC lathe work but have lots of experience with CNC mill. I'm creating my 1st few programs in Fusion for cutting on my Sherline Chucker lathe which is a gang tool lathe. With my current set up which will be a default set of tools I have my cut-off tool at the top of the gang tool table coming in from the top. in the picture, it is tool #9 at the very top. I am trying to figure out how to resolve an issue regarding the cut-off operation. The tool path will not generate because I have the tool orientation set to the tooltip coming in from the top. Ive changed every setting I can but no resolve. Including edge to base the cut on, tool tip side etc. When I change tool orientation to the standard from the bottom approach it generates the tool path fine.

IS there a special setup or considerations for gang tool lathe setup and tools coming from both front and back?

Here is the file 

https://a360.co/3tLETqA

 

[seth.madore]

What post processor are you using?
Most of the Post Processors have certain settings that allow for X+/X- tool settings and posted code. For example, on a Mach3 turning post processor, you can set your Turret value to 103 (tool library > Tool > Post processor) and that will give you code for an X- tool

"Use Turret 0 for Positional Turret, Turret 101 for QCTP on X- Post, Turret 102 for QCTP on X+ Post, Turret 103 for Gang Tooling on X- Post, Turret 104 for Gang Tooling on X+ Tool Post.";

[seth.madore]

So, in short, define all your tools as if you have a turret like a conventional lathe, all coming in from the proper direction. Fusion and the post processor will (should) handle the rest

[BillGEGHV]

Im on a Centroid control using an Acron control board. So yes the tool setup has the ability to set tool orientation, so that part is taken care of. I have not even ran the part with the cut-off tool because Fusion will not gen the tool path.

From what you are saying that means everything is happening on the back end, which is fine, but WHY is it that the tool path will not generate when I have the tool orientation set up (in Fusion tool library) for a top approach X+ move. The tool & holder is red like there is something wrong. SO Does this then mean I can not do simulations? I can never see the tool path for a visual reference and confirmation etc.

Not sure I understand what your saying here
"define all your tools as if you have a turret, like a conventional lathe,"
A conventional lathe would have a single tool holder or tool post tool holder, not a turret? Can you clarify what you mean here?

And ultimately are you also saying I need to edit the Gcode? 

[seth.madore]

No, editing the g-code is not needed.

"conventional lathe" = standard CNC lathe, turret that indexes as needed

Setup all your tools with the orientation that works for the selected tool. As you discovered, they will not work in the orientation they physically are in your machine. Ignore that, just get them to not be red. Your post processor is the Centroid, so reading the post a bit, we find:

"Generic turning post for Centroid. Use Turret 0 for Positional Turret, Turret 101 for QCTP on X- Post, Turret 102 for QCTP on X+ Post, Turret 103 for Gang Tooling on X- Post, Turret 104 for Gang Tooling on X+ Tool Post.";

So, in your parting tool, set the Turret value to 104 and it will get you code that is proper, and a simulation that mostly makes sense, assuming you can ignore that it's pointed opposite of what you actually are holding it.

FWIW, sub spindle work is the same way, I have to define RH holders, even though I'm using LH

[BillGEGHV]

Awesome thank you Seth, couple more Qs.

Would this (104 turret value) / addition to the tool parameters apply to all tools that are approaching from the top? I assume so? Right?

So for simulation, you just have to get used to it coming in from the bottom approach correct?

IS there any chance for the development team to add this to simulations? So you can see it comming in from top just for visual confirmations, tootip, toolside etc. Easer to visualize if its what the machine is set up like.

Is there any option to add the 104 value to the post "permanently" I have a terrible memory and when programming new tools Im sure I will forget to add that value? I realize it's a tool parameter but just figured Id ask.

[BillGEGHV]

Quite the setup and machine shop arsenal there at Liberty.     NICE setup man.      I have a Tormach. LOL, Maybe I get there someday.  

[seth.madore]

I'll answer these in no particular order:

1) Thanks, it's been a lot of work to get it to that stage. I also added a Doosan Lynx LSYB (twin spindle, C/Y axis lathe) and an automatic CMM. Also just expanded into another 1,400 sq/ft, so things aren't as tight as they used to be...

2) Yes, we are planning on eventually making things visually correct. It's on the long term roadmap, so you're going to have to use your imagination for quite some time I suspect

3) RE, adding 104. That's going to be entirely on you and your tool library. If your part off tool is always there, just change it at the library level so you don't have to remember each time you pull it into a job file

[billbarschdorf]

I changed the tool to the 104 value for the turret, but now I'm getting an an error "exceeding the travel in X". Any input how to resolve that? 

[seth.madore]

Where do you receive the error; at the machine or when post processing?

[billbarschdorf]

At the machine in the CNC12 Control when hitting cycle start. 

[billbarschdorf]

Hi Seth,  So turns out the Centroid post is not playing nice with the tool orientation.  I was able to post and run the grove and cut off tool with the standard tool orientation in the Fusion tool library setup.  When the program runs the tool movement is backward. 

I have a post on the Centroid Acorn forum related to another issue but also added info and questions regarding this to this issue of tool orientation.  Maybe you can take a look it has the details of my setup. Go to page 6 about 1/2 way down the page my post from Thursday Jan 27 11:39 to get the details and the response from Acorn users.  

https://centroidcncforum.com/viewtopic.php?f=60&t=6345&p=59671#p59671

Let me know what you think on this and IF there is a way to resolve it, a couple of users are just saying to program using Intercon (CNC12s conversational programming) BUT I would rather work in Fusion for both CAD and CAM. Ya eventually I will be learning intercon but for now need to get this worked out in fusion.  

CAN a custom post be made for me to resolve this? IF its needed? 

[russW4LXE]

Came over here after a suggestion from this other thread: https://forums.autodesk.com/t5/fusion-360-support/cam-reversing-tool-side-of-parting-tool-gang-tooli...

I am using a different post processor however for my Sherline Lathe as I am running LinuxCNC with Axis. I will attach the PP file I am using. 

Thanks in advance for any help.