The Top Round/Chamfer Milling Dialog Box
The Machining Strategy section of the Top Round/Chamfer Milling dialog box contains the following options.
Roughing
Rough Top Feature— Remove the material over the round or chamfer using rough milling and leaving stock on the Floor according to the Stock value (the stock is measured in the direction normal to the surface of the round or chamfer).
Finishing
• Finish Feature—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. All the increments are measured in the direction normal to the surface of the round or chamfer.
• 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. This option becomes available only when you select the Finish Feature option above.
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 round or chamfer, 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).
Connect Motions
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 Top Round/Chamfer 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.