G112 with Milling Toolpaths on VTL with X4

[JMWorks]

I need to mill some 3D surfaces in a part using our live tooled VTL. I tried posting what I had to see the code and it will not output a G112. I have the misc value #4 set to 1 like I have always used. This is on the surface high speed rough and finish waterline toolpaths that it will not work. It will output fine for the contour path I have in the part though. Also noticed some sort of a bug in verify while watching a tool run compared to the toolpath shown in backplot which is unhandy. Any thoughts?

[BrianCNC]

I haven't ever tried using G112 in a surfacing tool path, and I am assuming you don't have a Y axis. Is the work you are doing on the face of the part? According to my post the cuttype needs to equal four (Y axis substitution) or the abs(cuttype) needs to equal two (r/l face cut) in order for the millcc to be set equal to the misc value 4. I would suppose a post for a VTL would be set up in a similar way.

 

When using mill/turn verify and backplot seldom do the same thing.

[JMWorks]

Sadly, no Y axis but a full contouring C. Yes this is on the face of the part. I will look through the post a little bit later and check those values you had mentioned.

[BrianCNC]

I tried a radial finish toolpath with both a NL3000 set up and a vtl and both output the G112 (G12.1) code.

 

The current values for the cuttype variables will not be in the post, they'll come from the NCI file and change based on operation.

[JMWorks]

Brian please try a Surface High Speed path. I just tried a normal surface roughing path and was able to output the G112 correctly there so I am thinking that it just does not work with the Surface High Speed paths. I guess I will switch to a normal contour surface path, strange the High Speed paths will not work, I did not notice a difference in the paths just the amount of control I have over it. Thanks for the help!

[BrianCNC]

I did try the high speed tool path and it would not output the G112.

 

The conditions I explained here are necessary to set the millcc variable to 1 from the misc value, but another set of conditions come into play in order to output the G112 or G107. In the pmillccb post block the cutpos2$ needs to equal one in order to output an G112 and when I ran a high speed tool path the cutpos2$ was always zero.

 

1=Start point, first point on surface, chained contour, etc

 

0=Before start point; reset at each tool change, including null

 

 

So I would say the high speed surface tool paths do not support the G112 or G107 cycles.

[JMWorks]

Thanks for checking that out Brian. I am not as good with editing and reading posts and using the debugger yet as I should. I'm still finding new features in Mastercam everytime I actually get to use it and not need to hurry up and get a code out.

[BrianCNC]

Don't feel frustrated, it takes time. I am nowhere close to being as good as a lot of the guys on this forum are.

I know what you mean on not having any time to investigate anything. I tried all the above during lunch and after work.