To Create a Surface Milling NC Sequence
When you create a Surface 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 Surface Milling NC sequence.
1. Ensure that the current operation references a Mill/Turn workcell.
2. Click
Mill >
Surface Milling. The
SEQ SETUP menu appears.
The following surface milling specific commands are available on the SEQ SETUP menu in addition to the common commands for all NC sequence types.
◦ Tool—Select the tool that you want to use for the NC sequence.
|  If you want to create a surface milling NC sequence using a side milling tool, Creo NC does not allow you to select the side milling tool at this stage. However, continue the NC sequence with the default tool. While defining the cut, select the required option. After you define the NC sequence, click Seq Setup. On the SEQ SETUP menu, click Tools followed by DONE. In the Tool Setup dialog box that opens, select the side milling tool that you want to use for the NC sequence and click OK. |
◦ Surfaces—Select surfaces to be machined. If you are selecting quilt surfaces, specify which side of the surfaces you wish to machine.
◦ Window—Create or select a Mill Window. Appears for 3-Axis NC sequences only. This option and Surfaces are mutually exclusive. If you use the Window option, then all the surfaces within the specified Mill Window will be selected.
◦ Close Loops—Specify loops to close for Window machining. Appears for 3-Axis NC sequences only.
◦ ScallopSrf—Select surfaces that will be excluded from scallop computation if SCALLOP_HGT is specified.
◦ 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. Appears for 4- and 5-axis NC sequences only.
◦ 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 (or define a Mill Window).
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:
◦ From Surface Isolines—Mill the selected surfaces by following the surface u-v lines.
◦ Projected Cuts—Mill the selected surfaces by projecting their contours on the retract plane, creating a "flat" tool path in this plane (using the appropriate scan type), and then projecting this tool path back on the original surface(s). This option is available for 3 Axis Surface Milling only.
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. For more information on defining the cut using a particular method, follow the appropriate link under See Also. 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.