Mastercam Toolpath Transform Methods: NCI vs Geometry
Have you ever wondered what the differences are between using the NCIor Geometry options when transforming a toolpath? Here’s a quick primer.
The NCI option will copy and transform the source operation’s NCI lines. Mastercam reads each NCI line from each source operation, extracts all the values from each line, and transforms them based on the transform parameters.
It’s fast when the transform method is Coordinate; even faster when transforming by Toolplane.
For Translateand Rotate transforms, the NCI option is accurate, but there are many issues when using this option with Mirrortransforms, such as:
§ maintaining cutting direction
§ applying cutter compensation direction
§ avoiding creating invalid left-handed views
§ maintaining depth cut order
§ converting rapid retracts into feed moves
§ converting feed moves in Z into rapid moves
Contour and pocket toolpaths have their depth cuts marked as such in the NCI, but multi-surface toolpaths do not. This means that a mirror transform of a multi-surface toolpath with the Reverseoption selected would cut from bottom to top.
Use the Geometry method to copy and transform the source operation’s parameters, geometry, and toolpath references and to generate an entirely new NCI section.
This method copies and transforms the geometry needed for toolpath creation. The copied geometry is temporary when the Create new operations and geometry option is off, and permanent when that option is selected.
Geometry is the only mode available when mirroring operations. It may be slower to copy, mirror, and regenerate multi-surface toolpaths, but the resulting toolpath will be correct. The Geometry method ensures that all cutting directions, cutter comps, lead-ins and lead-outs, start points, etc., come out as if the user mirrored the geometry and programmed it manually. Wireframe toolpaths are quick and speed is not an issue.