To Create a Swarf Milling NC Sequence
When you create a Swarf Milling NC sequence, you are given a choice of several methods for defining the cut. Depending on the selected method, the tool path will be different. You can change the Cut Type (that is, select a different method of defining the cut and specify the new parameters and references) at any time when you redefine a Swarf Milling NC sequence.
1. Ensure that the active operation references a 5–axis Mill or Mill/Turn workcell.
2. Click
Manufacturing >
Milling >
Swarf Milling.
The SEQ SETUP menu appears with the required commands checked. The following swarf milling specific commands are available on the SEQ SETUP menu in addition to the common commands for all NC sequence types:
◦ Surfaces—Select surfaces to be machined. If you are selecting quilt surfaces, specify which side of the surfaces you wish to machine.
◦ Height—Specify a plane or surface for the tool tip to follow.
◦ Check Surfs—Select additional surfaces against which gouge checking will be performed.
◦ Define Cut—Define the method of surface milling and specify the appropriate parameters.
◦ Axis Def—Control the orientation of the tool axis.
◦ Build Cut—Access the Build Cut functionality.
◦ Approach/Exit—Specify the approach and exit moves.
The required options are selected automatically. Select additional options, if desired, and click Done. The system will start the user interface for all selected options in turn.
3. Select the surfaces to be milled.
4. When you start to define the cut, the system opens the Cut Definition dialog box. Specify a method of defining the cut by selecting one of the following options:
◦ Straight Cut—Mill the selected surfaces by a series of straight cuts parallel to the XY plane of the NC Sequence coordinate system. The cuts are spaced evenly along the z-axis in STEP_DEPTH increments.
◦ From Surface Isolines—Mill the selected surfaces by following the surface u-v lines. The user interface is similar to defining the cut for a Surface Milling NC sequence.
◦ Cut Line—Mill the selected surfaces by defining the shape of the first, last, and some intermediate cuts. When generating other cuts, the system gradually changes their shape to accommodate surface topology. The user interface is similar to defining the cut for a Surface Milling NC sequence.
Depending on the selected method, the system displays the appropriate options in the lower portion of the Cut Definition dialog box.
5. Select the appropriate options in the Cut Definition dialog box and specify geometric references to define the cut according to the selected method. When satisfied with the cut definition, click OK to close the Cut Definition dialog box and generate the tool path.
6. On the NC SEQUENCE menu, click Play Path to verify the tool path automatically generated by the system. Use the Customize functionality, if needed, to adjust the tool path.
7. Click Done Seq or Next Seq when satisfied.