The Slab Milling Dialog Box
The Machining Method section of the Slab Milling dialog box contains the following options.
Roughing
Rough Slab—Remove the material inside the Slab feature using rough milling and leaving stock according to the Floor Stock and Wall Stock values:
• Floor Stock—Stock to be left on the Floor surfaces.
• Wall Stock—Stock to be left on the Hard Walls.
Finishing
• 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.
• Back Off Walls—When you do rough milling and finish floors within the same tool path, you can keep the tool off the walls by a specified additional distance while the Floor is being finished. You can then finish the walls later. This option becomes available when both the Rough Slab and Finish Floors options are selected and the Finish Walls option is cleared. When you select this option, type the back-off distance in the text box to the right.
• 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.
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 Slab feature, moving back and forth. At the end of a pass, it retracts and moves to the beginning of the next pass, unless the Reverse Multiple Passes option is selected.
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. 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 Slab Milling dialog box contains the following options:
• Reverse Multiple Passes—If Back and Forth is selected, this option will reverse the Cut Angle on successive passes. Use this option to perform continuous back and forth machining between passes.
• 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.