To Create a Corner Finishing NC Sequence

1. Ensure that the active operation references a Mill or Mill/Turn Workcell.

2. Click Mill >

Corner Finishing.

3. Select

, or

for finishing on Head 1, Head 2, Head 3, or Head 4.

The Head Selector options are available only if the operation references a Mill-Turn or Lathe, and if both heads are activated in the work center.

4. Click

Tool Manager or select

Edit Tools from the tool list box to open the Tools Setup dialog box and add a new cutting tool or change tool parameters. The tool list only includes tools that are valid for the step.

To show tools for the current step and the active head on the machine tool, set the INCLUDE_ALL_TOOLS_IN_LIST option to YES.

Alternatively, right-click in the graphics window and select Tools.

5. To preview the cutting tool and its orientation in the graphics window, click

adjacent to the right of the tool list box. The

button becomes available once a tool is selected.

Alternatively, right-click the graphics window and select the Tool Preview option on the shortcut menu. After you select a tool, the Tool Preview option is available on the shortcut menu of the graphics window.

To exit the tool preview, right-click the graphics window and select Cancel tool preview from the shortcut menu.

6. To change the coordinate system that defines the orientation of the step, click the collector adjacent to

and select a coordinate system. If the operation coordinate system differs from the step coordinate system, right-click the collector for the following options:

◦ Default—Replaces the selected coordinate system with the default reference. The default is the orientation that is copied from the previous step or from the operation.

◦ Information—Displays the information of the selected coordinate system.

After you specify a coordinate system for an NC sequence, it remains in effect until you change it.

Alternatively, right-click the graphics window and select Orientation from the shortcut menu.

7. Select the following options on the References tab:

◦ Reference Cutting Tool—Select or define the reference tool, which must be a ball end mill. This is used to calculate the remaining area.

When you set the STEEP_AREA_SCAN and SHALLOW_AREA_SCAN parameters to PENCIL_CUT, Creo NC calculates the tool path without considering the previous tool.

◦ Machining Reference—Create a mill window or select one from the graphics area or model tree. All the corners within the specified mill window are machined.

To create a new mill window, click

Geometry >

Mill Window on the Corner Finishing tab. See Related Links for more information on creating a Mill Window.

◦ Excluded Surfaces—Select surfaces that lie inside the mill window that you want ignored while machining.

The Excluded Surfaces option is available on the References tab and the shortcut menu of the graphics window, only when you select a machining reference.

Alternatively, right-click the graphics window and select Excluded Surfaces, Machining Reference from the shortcut menu.

8. On the Parameters tab, specify the required manufacturing parameters.

You can also click

to copy parameters from an earlier step or click

to edit parameters specific to Corner Finishing. By default, the required parameters are defined by relations that you can modify from the Relations dialog box.

Alternatively, right-click the graphics window and select Parameters from the shortcut menu.

9. On the Clearance tab, optionally specify the following:

◦ Retract—Specify the Type, Reference, Orientation, and Value for the retract definition

◦ Start and End Points—Specify the Start point and End Point for the step tool path.

Alternatively, right-click the graphics window and select Retract. You can also select the Start Point and End Point of the cutting tool from the shortcut menu.

10. On the Options tab, open a part or assembly to use as a cutting tool adapter. Alternatively, click

to copy cutting tool adapter from another step.

11. Select options on the Tool Motions tab to create, modify, and delete tool motions and CL commands for defining cut motions. For details on all the tool motions, see the topics under Related Links.

Alternatively, right-click the graphics window and select Tool Motion Options.

The Return to Step Options option on the shortcut menu in the graphics window enables you to switch from editing tool motions and editing step reverences. This option is available only when all references for tool path computation are successfully defined.

12. Click

to get a dynamic preview of the tool path in the graphics window.

13. On the Process tab, optionally use any of the following options for the machining step:

◦ Calculated Time—Click

to automatically calculate the machining time for the step. The Calculated Time box shows the time.

◦ Prerequisites—Click

. The Select Step dialog box opens. Select an existing step that is a prerequisite for the new roughing step. Click OK.

The Prerequisites option is available on the Process tab while creating or editing a step from the Process Manager.

14. On the Properties tab, optionally specify the name or comments for the step.

◦ Name—Displays the name of the step. You can type another name.

◦ Comments—Type the comments associated with the step in the text box or use the following options:

▪

—Read in an existing text file containing step comments and replace any current step comments.

▪

—Insert the contents of an existing text file of step comments at the cursor location. Preserve any current step comments

▪

—Save current step comments in a text file.

▪

—Accept the current step comments.

15. After you define the mandatory step elements, the following buttons become available:

◦ To play the tool path, click

◦ To perform gouge checking against surfaces of the reference part, click

◦ To view the simulation of material removal as the tool is cutting the workpiece, click

. The Material Removal tab with integrated simulation environment opens.

16. Select one of the following options to complete the sequence:

◦ Click

to save the changes.

◦ Click

to pause the process and use one of the asynchronous tools. Click

to resume.