The Through Slot Milling Dialog Box
The Machining Method section of the Thru Slot Milling dialog box contains the following options.
Roughing
Rough Slot—Remove the material inside the Slot feature using rough milling.
Finishing
• 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. This option becomes available only when you select the Finish Walls option above.
Cut Motion
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).
Start Position
This group of options can be used only if the Through Slot feature is completely surrounded by Hard Walls. If the Through Slot feature contains a chain of Soft Walls (there can only be one such chain), then the start position is determined automatically based on the Soft Wall location and the Climb/Conventional setting.
If the Through Slot feature is completely surrounded by Hard Walls, then when you select the Finish Walls option, the Start Position group of options becomes available.
If the Use Default option is selected, the tool will start at a default position along the through slot.
If you clear the Use Default checkbox, you can click 
next to it and select a point anywhere on the edges surrounding the through slot. The tool will start at the position closest to the selected point. Click 
to view the start position.
next to it and select a point anywhere on the edges surrounding the through slot. The tool will start at the position closest to the selected point. Click to view the start position.Top Entry
These options describe the way the tool enters the slot:
• 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 tool).
• 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.
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.