The Through Pocket Milling Dialog Box
The Machining Method section of the Through Pocket Milling dialog box contains the following options.
Wall Machining
• Rough—Remove material inside the pocket using rough milling and leaving stock on the walls of the pocket according to the Rough to value.
• Finish—Finish mill the walls of the pocket. 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 way the tool scans the horizontal cross-sections of the pocket:
• One Direction—Cuts in one direction only. At the end of each cutting pass, the tool retracts and returns to the opposite side if the pocket, to start the next pass in the same direction.
• Back and Forth—Continuously machines the pocket, moving back and forth.
• 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.
Clean Up Cut—Cleans up the walls of the pocket 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.
Top Entry
These options describe the way the tool enters the pocket:
• Plunge—The tool enters the material vertically.
• Ramp—The tool enters at Ramp Angle to the x-axis of the Program Zero coordinate system. You can customize the Ramp Angle by clicking the Tool Path Properties button and using the Entry/Exit tab of the Tool Path Properties dialog box.
• Helix—The tool enters along a helical path. You can customize the helical entry by clicking the Tool Path Properties button and using the Entry/Exit tab of the Tool Path Properties dialog box. Type the new values for the Helix Angle and the Radius of helix (the default for which is calculated by the system based on the size of the part).
• Entry Hole—The tool enters along a predefined entry hole. To use this option, you must first create and machine an Entry Hole feature for this pocket.
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 Through Pocket 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.