Back-Turning in Mastercam Lathe 2018

[bbeauregard]

Anyone have any experience with custom tools in MasterCam lathe 2018? I'm trying to create a back-turning tool. I drew a .125 wide back-turning tool (Sandvik Corocut xs #MABR 3 020 125) but I'm having issues with the toolpaths. I can cheat and make it work by adding a couple of lines and creating a groove on my part but I would like to get it to work like a standard turning tool.

Thanks for your help!   

[crazy^millman]

2 hours ago, bbeauregard said:

Anyone have any experience with custom tools in MasterCam lathe 2018? I'm trying to create a back-turning tool. I drew a .125 wide back-turning tool (Sandvik Corocut xs #MABR 3 020 125) but I'm having issues with the toolpaths. I can cheat and make it work by adding a couple of lines and creating a groove on my part but I would like to get it to work like a standard turning tool.

Thanks for your help!   

Can you share a file? I have done back turning back to V9 with little issue. You should be able to bring in the solid of the tool in 2020 and be off to the races. What Version are you using?

[bbeauregard]

I don't have a solid of the tool. I drew it in mastercam based on measurements I took of the insert. I am using Lathe 2018. I should point out that I am using lathe default but for a Citizen swiss lathe. I draw on the right hand side to get "Z" moves in the plus direction which is how Citizens are set up.  

[crazy^millman]

6 minutes ago, bbeauregard said:

I don't have a solid of the tool. I drew it in mastercam based on measurements I took of the insert. I am using Lathe 2018. I should point out that I am using lathe default but for a Citizen swiss lathe. I draw on the right hand side to get "Z" moves in the plus direction which is how Citizens are set up.  

Then are you exporting the tool to a level from the lathe tool manger that is close to what you need and then using that as the roadmap to duplicate it?

[bbeauregard]

So I created the tool based on a training tutorial I found online, I believe its from Mastercam. They have you draw a tool on level 111 then from the lathe tool manager you "create new tool" "custom" then enter the geometric tool orientation, tool geometry, tool orientation in turret, corner radius, tool center, and compensation. 

[crazy^millman]

53 minutes ago, bbeauregard said:

So I created the tool based on a training tutorial I found online, I believe its from Mastercam. They have you draw a tool on level 111 then from the lathe tool manager you "create new tool" "custom" then enter the geometric tool orientation, tool geometry, tool orientation in turret, corner radius, tool center, and compensation. 

Not the best way to do it in my humble opinion. Take an existing tool and then in the lathe tool manager right click and save to level use that to help you road map what your after. Too many ways to make mistakes staring from scratch. By using an existing tool you have a much better chance to get it correct. Then use that new level tool to make the custom tool and I think you will be golden.

[bbeauregard]

That does sound much easier. I'll give it a shot tomorrow. Thanks for your help!

[bbeauregard]

So I was able to create the tool no problem with the method above but I'm having a similar problem as before where I get a "Toolpath starts with the tool embedded in the stock" error. By changing some setting in the tool path I can get it to run through put then the tool cuts in places it should not.

[crazy^millman]

22 hours ago, bbeauregard said:

So I was able to create the tool no problem with the method above but I'm having a similar problem as before where I get a "Toolpath starts with the tool embedded in the stock" error. By changing some setting in the tool path I can get it to run through put then the tool cuts in places it should not.

If you know it is right then turn off stock update and that might fix the issue.

[nickbe10]

On 2/21/2020 at 2:34 PM, bbeauregard said:

By changing some setting in the tool path I can get it to run through put then the tool cuts in places it should not.

Sounds like you have a conflict with your tools and offset direction.

For normal turning you use a right hand tool offset to the right.

For back turning it would be a left hand tool offset to the left. not having this correct will result in the condition you describe.

Also make sure the tool is oriented properly in the set up page.

[bbeauregard]

Here is some pictures of whats happening and how the tool is setup. In the picture of the part the yellow line is what I want to back-turn, the blue line is where it's going to which is above where I want to make a finish path. I will post the other pictures separate, it won't let me post all of them together. 

[bbeauregard]

Here is tool setup pic #1

[bbeauregard]

Here is tool setup pic #2

[bbeauregard]

And here is tool setup pic #3

[crazy^millman]

Throw up a file and someone can better get an idea what your trying to do. Have you reached out to your dealer?

[bbeauregard]

Finally got it to work. Took a little experimenting but after turning off the stock update and playing around with orientation as stated above its cutting as it should. Posted code and that looked good too. Needed to change the orientation in both top plane and turret to #6. Thank You! 

[nickbe10]

11 hours ago, bbeauregard said:

Finally got it to work.

Whenever you see the cut or rapid line go south like that, tool orientation should be the first port of call, everything has to work together.