The Undercut Milling Dialog Box
The Machining Strategy section of the Undercut Milling dialog box contains the following options.
Roughing
Rough Undercut—Remove the material inside the Undercut feature using rough milling and leaving stock according to the Ceiling/Floor Stock and Wall Stock values:
• Ceiling/Floor Stock—Stock to be left on the Ceiling and Floor surfaces.
• Wall Stock—Stock to be left on the Hard Walls.
These options define the number of cutting passes:
• Multiple Cuts—The tool makes multiple cutting passes, machining away all the material and leaving stock on the Ceiling and Floor surfaces according to the Ceiling/Floor Stock value. The first cutting pass is at the top of the Undercut (taking into account the Cutter Width of the tool and the ceiling stock value). You can control the distance between the passes by using the Depth of Cut option, located on the Cut Control tabbed page of the Tool Path Properties dialog box.
• Single Center Cut—The tool makes only one cutting pass, leaving equal amounts of material on the Ceiling and Floor surfaces. If you select this option, the Ceiling/Floor Stock text box becomes unavailable, because the amount of stock left on the Ceiling and Floor surfaces is determined by the Cutter Width parameter of the tool.
Finishing
• Finish Ceiling/Floor—Finish mill the Ceiling and 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.
• 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 direction:
• One Direction—The tool cuts in one direction only. At the end of each cut, the tool returns to the opposite side, to start the next cut in the same direction.
• Back and Forth—The tool continuously machines the Undercut, moving back and forth.
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).
Motion Between Cuts
These options describe the way the tool makes the horizontal connections between the cutting motions:
• Clear Part—The tool clears the Soft Walls when exiting and entering the material for each cut.
• Stay in Cut—The tool stays engaged in material between cuts.
These options describe whether the tool retracts when connecting the cutting motions:
• Stay Down—The tool does not retract between the cut motions.
• Retract—The tool retracts at the end of a cut motion and goes to the beginning of the next cut motion at retract height (as defined by the Clearance tab of the Tool Path Properties dialog box).
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 Undercut 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.