The Freeform Milling Dialog Box
The Drive Geometry section of the Freeform Milling dialog box contains the following elements.
• Program Zero—Change the coordinate system used for machining, if desired.
• Drive Geometry—Define the tool trajectory in the XY-plane of the Program Zero coordinate system:
◦ Use Model Edges—Select edges from the reference model or from the stock.
◦ Sketch—Sketch the trajectory of the tool in the XY-plane of the Program Zero coordinate system.
• Cut Depth—Define the height of the last tool pass.
The Machining Method section of the Freeform Milling dialog box contains the following options.
Direction of Cut
These options are available when you define Drive Geometry by selecting model edges. They 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).
Tool Side
These options are available when you define Drive Geometry by sketching. They define where the tool is relative to the sketch:
• Left—The tool is to the left from the sketch.
• Right—The tool is to the right from the sketch.
• On—The tool follows the sketch. Use the Material Side options to specify cutter compensation.
Material Side
These options define how to apply cutter compensation when the tool follows the sketch:
• Left—Material is to the left.
• Right—Material is to the right.
Cut Ordering
These options define the order of machining if you specify multiple cuts and passes:
• X-Y First—The tool makes all the cuts at a specific depth and then moves to the next depth.
• Z First—The tool makes multiple passes to depth and then goes to the next cut.
The Multiple Cuts button opens the Finish Cuts dialog box, where you can set up the number and depth of finish cuts.
The Multiple Passes button opens the Finish Passes dialog box, where you can set up the number of finish passes and the depth increments.
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 Freeform Milling dialog box contains the following options:
• 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.
• 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.