The Pocket Milling Dialog Box

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

Rough Pocket—Remove material inside the pocket using rough milling and leaving stock according to the Floor Stock and Wall Stock values:

• Floor Stock—Stock to be left on the Floor of the pocket.

• Wall Stock—Stock to be left on the walls of the pocket.

• Finish Floors—Finish mill the Floor of the pocket. 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 pocket 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 Pocketand 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 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.

• Corners Only—Clean up the corners with a smaller tool after removing material from the pocket with a large tool.

• 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.

• One Direction—Cuts in one direction only. At the end of each cut, the tool retracts and returns to the opposite side of the pocket, to start the next cut in the same direction.

• Back and Forth—Continuously machines the pocket, moving back and forth.

• Spiral—Generates a spiral cutting path.

• 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.

• 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.

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.