The Profile Milling Dialog Box
The Machining Method section of the Profile Milling dialog box contains the following options.
Wall Machining
• Rough—Remove material using rough milling and leaving stock on the Hard Walls according to the Rough to value.
• Finish—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 cutting pass, the tool returns to the opposite side, to start the next pass in the same direction.
• Back and Forth—The tool continuously machines the Profile feature, 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).
These options define the cutting direction:
• Follow Hard Walls—The tool follows the shape of the Hard Walls.
• Straight Line—The tool cuts straight at a constant angle to the Program Zero coordinate system.
Cut Angle—Defines the angle between the cut direction and the x-axis of the feature-level Program Zero coordinate system if Straight Line is selected. 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.
Clean Up Cut—Cleans up the Hard Walls after the rough cut and before the finish cuts, to remove scallops left by the rough cut. Type the value for the minimal amount of stock to be removed by this cut in the Stock text box to the right.
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 Profile 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.