Converting arcs to lines

[SnahOlah]

Does anyone know a way to convert arcs to lines using toolpath parameters like filtering etc. I know I can actually break the arcs using break many but I'd rather be able to do it from the toolpath (or some other way?). I also should mention the "present arcs as lines" setting in smoothing doesn't appear to do it. And a somewhat related question (at least in my case) does anybody have good advice for cases with surface finish toolpaths where the tool moves up and down in z very slightly (0.0002 or so ) and you want to round that off to no z motion? Thanks in advance...

[Colin Gilchrist]

Why not just turn off Arc Support in the Control Definition, and force Mastercam to Linearize everything? Same goes for the Toolpath filters, you can enable the Filter, set a tolerance, and just don't enable the "Line/Arc" Filter.

If you drive an Arc (wireframe) as part of a Contour Path, you'll get a G2/G3 Arc in your NC Code, unless you disable the Arc Support in the Control Definition.

If you want to be able to "choose" which paths get Linearized, and which ones are allowed to output Arcs, then you need to make some post modifications. The variable 'linarc$' can be set inside the Post to force Arcs to be linearized by the Post itself. It is pretty easy to tie that into a Misc Integer or Real Number, to give you control over the output to your NC Code.

Your Reseller would be the first place to go for help with this... 

[SnahOlah]

As far as I can see turning the filter on without arcs selected (or leaving it off) still yields arc output (may still be missing something). The post edit you mentioned seems reasonable but I would only do that after I conclude I can't do this another way. And I do want to only apply this in certain cases so I'd rather not handle it in the control def. Do you know of a way using the filter / tolerances? Thanks for your help

[Colin Gilchrist]

If the "Input" geometry to the Toolpath contains Arcs, then no, there is no way to support Linearization of a path using "only" the Filter settings. If the Toolpath is based on Surface Machining Paths, then it is "point-to-point" by default.

The Control Definition would be the "Global" setting for Arc Support. If you disable it in the Control Definition, then every single path would always be Linearized, and you'd never get Arcs.

The only way to be able to control this using "as needed" options would be to use the Miscellaneous Integers to "pass" data to the Post Processor (for example, to select '0' for the conversion to be "off", or '1' when you want it to be "on" for an individual Toolpath). Then by writing logic in the Post Processor, you can determine when to output Arcs, and when they should be Linearized, using the 'linarc$' variable, along with 'chord_tol$' to control the breaking tolerance.

[Gracjan aka Pullo]

Put linarc = 1 into your postprocessor.

 

Gracjan