The Face Milling Dialog Box
The Machining Method section of the Face Milling dialog box contains the following options.
Machining Mode
• Rough—Face down the stock and leave stock according to the Rough to value.
• Finish—Finish mill the reference model surface(s). When you select this option, you can use the Finish Passes button to set up the number of finish passes and the depth increments.
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 Face feature, moving back and forth. At the end of a pass, it retracts and moves to the beginning of the next pass, unless the Reverse Multiple Passes option is selected.
• Spiral—Generates a spiral cutting path.
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).
Cut Angle—Defines the angle between the cut direction and the x-axis of the Program Zero coordinate system for One Direction and Back and Forth cut motion types. The default is 0, which means that the tool cuts parallel to the x-axis of the Program Zero coordinate system. To change the cut direction, type the new value in the Cut Angle text box.
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.
• Clear Part On Last Cut—If Stay in Cut is selected, this option will make the tool clear the part on the final cut of each pass.
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 Face Milling dialog box contains the following options:
• Reverse Multiple Passes—If Back and Forth is selected, this option will reverse the Cut Angle on successive passes. Use this option to perform continuous back and forth machining between passes.
• 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.