To Insert a Milling Step
To insert a new Milling step in a Process Table, you have to be in a Process view. You also have to have at least one operation defined in the process. Face milling, Profile milling, Trajectory milling (2-axis and 3-axis), Roughing, Reroughing, Finishing, Corner Finishing, Manual Milling Cycle, and Drilling steps can be defined completely within the Process Table. For other types of steps, the system starts the regular user interface for defining an NC sequence.
1. Select the line in the Process Table where you want to insert the new step and click . The Create Milling Step dialog box opens.
2. Type the name of the new Milling step in the Name box, to replace the default system name.
3. Select the type of the Milling step. The following types are available:
TRAJECTORY MILLING (3- to 5-axis Trajectory milling)
CURVE TRAJECTORY (2-axis Trajectory milling)
4. Select the number of axes in the Axis box, if needed. The number of axes that you can select is limited to the number of axes in the parent workcell and the type of milling step.
You cannot change the axis number in the Axes cell while editing any milling step.
5. Select Head1 or Head2 in the Head box to specify the milling head to be used for the NC sequence (Head1 is the default). Head1 and Head2 are available only when you select the Milling option for both the heads in the Machine Capabilities dialog box.
The options in the Head box of the Create Milling Step dialog box are available only if the workcell type is a 4- or 5-axis Mill-Turn center.
6. Click OK. The tab for the selected milling step opens. For example, if you create a Profile Milling step, the Profile Milling tab opens.
The milling tab also opens when you click on the toolbar below the Process Table to edit the step.
A milling tab has the following additional tabs:
7. References—Lets you select a machining reference. For Face milling, Trajectory milling and Profile milling, you can select geometric references for the step, such as surfaces to machine and scallop surfaces.
For Roughing, Reroughing, Finishing, and Corner Finishing steps, the following additional options are available:
Lets you select a mill window for the step. The mill window is mandatory for all but Reroughing steps.
For Roughing and Finishing, lets you select the loops to close for machining. Creo NC does not create the tool path in the selected loops.
For Finishing and Corner Finishing, lets you select surfaces from the reference model, that you want Creo NC to ignore while machining.
For Face milling, 2-axis Trajectory milling (step type CURVE TRAJECTORY), Manual Milling Cycles, Roughing, Drilling, Profile milling, and 3-axis Trajectory milling, lets you specify a start point and end point for the step.
8. Parameters—Lets you specify the required manufacturing parameters.
You can also click to copy parameters from an earlier step or click to edit parameters specific to the milling step. 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. Clearance—Lets you 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.
10. Tool Motions—Lets you create, modify, and delete tool motions and CL commands for defining cut motions. Alternatively, right-click the graphics window and selectTool Motion Options.
11. Options—Lets you open a part or assembly to use as a cutting tool adapter. Alternatively, click to copy cutting tool adapter from another step.
For Profile milling, enables you to select the approach and exit axis for the profile milling slices.
12. Check Surfaces—Lets you define the parts and surfaces that can be used as a limit on the tool motions during machining.
Alternatively, right-click the graphics window and select Check Surfaces.
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.
Actual Time—Specify the machining time.
Prerequisites—Click . The Select Step dialog box opens. Select an existing step that is a prerequisite for the new milling step. Click OK.
14. On the Properties tab, optionally specify the name or comments for the step.
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 inserting the step:
Click to save the changes.
The system inserts a new step line below the selected line in the Process Table.
Click to pause the process and use one of the asynchronous tools. Click to resume.
Click to cancel the changes.