The Channel Milling Dialog Box
The Machining Method section of the Channel Milling dialog box contains the following options.
Roughing
Rough—Remove the material inside the Channel 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 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.
• 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.
Cut Motion
These options define the cut direction:
• One Direction—The tool cuts in one direction only, following the trajectory of the Channel feature. At the end of each cut, the tool returns to the opposite side, to start the next cut in the same direction.
• Back and Forth—The tool continuously machines the Channel feature, following its trajectory and moving back and forth.
• Spiral—Generates a cutting path where the tool starts from one Soft Wall, cuts down the center of the Channel, and then makes alternating cuts to the left and to the right from the first cut. When necessary, the cuts follow the Hard Walls to remove all the material inside the Channel feature. Use this option if the walls of the Channel feature are not parallel, or if it has more than two Soft Walls.
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).
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).
Start Wall
• Automatic—The Soft Wall where the tool starts cutting the material is chosen automatically. Click
next to the option to display the current Start Wall.
• Select—Select the Soft Wall where the tool starts cutting the material. Click
next to the option to select the Start Wall.
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 Channel 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.