engraving on a flat surface from the "x direction" on a live tooling lathe without y axis

[jeff2HS8X]

as the title says, I am trying to engrave some text on a flat surface of a part from the machines "x direction" (if that makes sense) on a live tooling lathe that does not have y axis .   basically, we have a part that we will mill a hex feature, and then i need to engrave some text on one of the flats. I have attached a screenshot and a .f3d file that will explain better what i am trying to do.  

I am planning to engrave the text with a small 1/32" ball end mill. the machine would need to move the c,x, & z axis all simultaneously for this to work. i have tried a couple different approaches and am not having any luck, and since i am using a ball mill and only plan to engrave about .005" axially into the flat, it should be entirely possible. maybe this is something that the software isn't capable of yet?

[seth.madore]

no, this is not possible in the software, as it will always be looking for a Y axis

[craig.chester]

If you define the toolaxis = TO CURVE...... and your curve is a straight line which is aligned to the rotary axis. Does this provide a solution? Theoretically, it'll not need a Y axis.

[seth.madore]

No, you're correct. However, I'm drawing a blank on what toolpath is available to the general subscriber that will do as you suggest. I know of some Previews we have access to that permit this, but not so much for the rest of the community

[craig.chester]

If the user has the Machining Extension, it may be possible to use the PROJECT strategy with the suggested tool axis settings? A single line (centreline) font would need to be used.

As stated, I haven’t tried this, but this is what I would try if time allowed.

[jeff2HS8X]

well if you remember and wouldn't mind sharing that would be great, i did enable the machining extension for this part with hopes that there is a toolpath that works...

Thanks,

[jeff2HS8X]

yeah you are right that, theoretically, this is entirely possible without a Y axis, its just a matter of the CAM understanding that as well

[seth.madore]

@craig.chester thanks for the prodding, that did the trick:

 

Now to see if I can get it to post out..

[seth.madore]

Looks like we have a winner!

Using the stock Doosan Turn/Mill post and setting it to "Lynx" (not "Lynx with Y"), it posts out without any Y moves.

I've attached the file for your review

 

[jeff2HS8X]

Seth, its looking like we are on to something! however, i loaded your file, and i have installed the doosan post with lynx enabled. its giving me an error

Error: Error: Direction is not supported for machine configuration.

Error at line: 1

Error in operation: 'Project3'

it does simulate perfectly though

[seth.madore]

Interesting. Try this post.

(Note; This is a post that I've been picking away at for my Lynx, there are some differences, but nothing ground-breaking)

[jeff2HS8X]

hmmm, that one is giving me same error as well. are you able to post out good code?

[seth.madore]

Yep, see attached file