Toolpath control of Fanuc AICC settings?

[DS_P]

Hey,

Right now I use a slightly tinkered version of the Fanuc post revision 44116 (added a few machine specific M codes but otherwise stock).

Currently AICC (G5.1 Q1) sets its R value based on a post processor property.  (for people searching this function is similar to Haas G187)

This works fine for 90% of what I do, but occasionally when running parts with very small radius's followed by short straight line segments, the AICC will create waves in the parts until it settles down (I think this is because AICC is actually converting small line segments into arcs in the control instead of following the straight line). I've tried just about everything machine side to stop it (for example at level 10 and very slow feed rates it still occurs), so would rather just turn it off occasionally.  

Anyways, what I'd ideally like to do is instead of setting AICC on/off/level property globally per program, it would be nice to control it on the tool path level.  I swear I once saw a video of someone with some customization that allowed each toolpath to have a new Post Process tab after Linking, with custom options.  Maybe I imagined it because I cant find any documentation on how to add custom post properties to each tool path. Any ideas?   If I can figure out how to do this I can probably modify the post to pick this value up per toolpath.

I've also seen it done where the post picks up the smoothing or tolerance value and makes a decision of R1 to 10 based on that, but really I'd rather manually set it myself (for example if its a large part with tight tolerance I might use R10, but if it a small part I'd have it off).

[DS_P]

Ok so kept looking and started to find what I was looking for after making this post. "Operation Properties" might be what I'm looking for (see post processor guide snips below).  Will experiment and report back.

[a.laasW8M6T]

Yep that's exactly what you want, 

I've done this on several posts and it works well.

If you run into trouble attach the post here and we can take a look

[DS_P · Accepted solution]

Yeah so I just solved this myself....

Here is the trick and its SO much easier to implement than I expected. Change smoothing scope from "post" to "operation."  After this is done, upload the post, attach it to your machine configuration.  Then in your Setup/ Machine selection, remove and re select your machine. If it worked it gives a warning about added properties. But then you get this per toolpath:

 useSmoothing: {
    title      : "Use smoothing",
    description: "Defines the smoothing control mode (AICC/AIAPC). 'On' outputs G05.1 Q0/Q1 only, 'Automatic' or 'Level 1-10' outputs G05.1 Q1 with the R value for the desired level.",
    group      : "preferences",
    type       : "enum",
    values     : [
      {title:"Off", id:"-1"},
      {title:"On", id:"0"},
      {title:"Automatic", id:"9999"},
      {title:"Level 1", id:"1"},
      {title:"Level 2", id:"2"},
      {title:"Level 3", id:"3"},
      {title:"Level 4", id:"4"},
      {title:"Level 5", id:"5"},
      {title:"Level 6", id:"6"},
      {title:"Level 7", id:"7"},
      {title:"Level 8", id:"8"},
      {title:"Level 9", id:"9"},
      {title:"Level 10", id:"10"},
    ],
    value: "-1",
    scope: ["operation"], // DSP edit 241008, changed from post to operation and limied to milling/ not drilling
    enabled: "milling", //DSP scope limiting to milling
    disabled : "drilling" // DSP Not displayed for drilling operations

For safety it is probably best to limit the scope to "Milling."  You will get errors on Fanuc if Drilling has AICC codes. There may be other toolpaths or codes on the Fanuc control where this is undesirable, will experiment.