The Slot Milling Dialog Box

The Machining Method section of the Slot Milling dialog box contains the following options.

Rough Slot—Remove the material inside the Slot feature using rough milling and leaving stock on the Floor according to the Floor Stock value. Stock left on the Hard Walls depends on the Advanced Slot Milling options selected.

• Finish Floors—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.

• 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.

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).

• 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 slot.

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.

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.

The Advanced Slot Milling section of the Slot Milling dialog box contains the following options:

• Single Center Cut (default)—The tool performs a single cut along the center of the slot. When you use this option, the amount of material left on the walls of the slot depends on the difference between the width of the slot and the cutter diameter of the tool.

• Multiple Cuts—The tool performs multiple cuts to remove the material inside the slot. Use the Wall Stock text box to specify the stock allowance left on the Hard Walls of the slot. When you use this option, the following additional options become available:

◦ One Direction—The tool cuts in one direction only. At the end of each cut, the tool retracts and returns to the opposite side if the slot, to start the next cut in the same direction.

◦ Back and Forth—The tool continuously machines the slot, moving back and forth.