The Flange Milling Dialog Box
The Machining Method section of the Flange Milling dialog box contains the following options.
Roughing
Rough Flange—Remove the material inside the Flange feature using rough milling and leaving stock according to the Floor Stock and Wall Stock values:
• Floor Stock—Stock to be left on the Floor surfaces.
• Wall Stock—Stock to be left on the Hard Walls. If the Flange feature does not have Hard Walls, this text box will be unavailable.
Finishing
• Finish Floors—Finish mill the Floor surfaces. When you select this option, you can use the Finish Passes button to set up the number of finish passes and the depth increments.
• Finish Walls—Finish mill the Hard Walls. When you select this option, you can use the Finish Cuts button to set up the number of finish cuts and the depth increments. If the Flange feature does not have Hard Walls, this option and the Finish Cuts button will be unavailable.
• Use CUTCOM—NC output will contain the CUTCOM statements. You can customize their format and locations by clicking the Tool Path Properties button and using the Cut Control tab of the Tool Path Properties dialog box.
Cut Motion
These options define the cut motion pattern:
• Follow Outer Contour—The tool follows the outer contour of the Flange.
• Follow Inner Contour—The tool follows the inner contour of the Flange.
These options define where material is relative to the tool rotation:
• Climb—The tool is to the left of material (assuming clockwise spindle rotation).
• Conventional—The tool is to the right of material (assuming clockwise spindle rotation).
Start Location
These options describe where the tool starts cutting:
• Start From Outer Contour—The tool starts at the outer contour of the Flange and moves inward.
• Start From Inner Contour—The tool starts at the inner contour of the Flange and moves outward. This option is not available if the inner contour is comprised of Hard Walls.
The Tool Path Properties button opens the Tool Path Properties dialog box, which provides access to lower-level control of the tool path, such as spindle and coolant statements, speeds, feeds, clearances, entry/exit, and cut control options.
The Options section of the Flange Milling dialog box contains the following option:
Use Fixture Offset—Allows you to store the fixture transformation offset in a register on your machine. Type the Fixture Offset register value in the text box to the right. If you use this option, NC output will contain the SET/OFSETL statements.