To Create an NC Sequence
You can create an NC Sequence by using options on the tab of the sequence you are creating. For example, to create a Profile Milling sequence, click Mill > Milling. The Profile Milling tab that enables you to define the tool path appears. Perform the required operation using options on the tab to create the sequence.
You have to set up an operation before creating an NC sequence where only one operation is active at a time. The type of work center defines the types of NC sequences you can create using the Mill, Turn, and Wire EDM tabs. Once you select the type of the NC sequence, define the tool path using options on the required tab.
The following generic tabs and buttons are available for creating an NC sequence:
Tool Button and the . Tool List
To select a tool or change tool parameters, open the Tools Setup dialog box in one of the following ways:
Select a tool from the tool list box, or click Edit Tools in the list box. The tool list box 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.
Click .
Right-click the graphics window and select Tools from the shortcut menu.
—Coordinate System Button
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 commands:
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.
Machining References Tab
Use options on this tab to specify geometry to be machined. A machining reference may be geometry from the reference model or workpiece, or manufacturing geometry created in the NC Assembly.
—Cutting Tool Preview Button
To preview the cutting tool and its orientation in the graphics window, click 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.
Parameters Tab
Use options on this tab to specify the required manufacturing parameters for an NC step.
Click to copy parameters from an earlier step or click to edit parameters specific to profile milling. 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.
Clearance Tab
Specifies the minimum distance by which the reference model, workpiece, and fixture components will be cleared during machining. Use the following clearance options:
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.
Check Surfaces Tab
Use the following options on this tab to define the parts and surfaces that can be used as a limit on the tool motions during machining:
Add Reference Parts—Add the reference parts used in the assembly to be checked.
Use Mill Stock Allowance—Specifies that the mill stock allowances defined should be considered to keep a safe distance from the machining. This distance is the same as the stock allowance for machined surfaces. If you do not specify the mill stock allowance, the CHECK_SRF_STOCK_ALLOW parameter is applied by default.
Check Surfaces Collector—Specifies parts and surfaces the cutting tool will check against during tool path computation. The tool path will be trimmed automatically to not violate these surfaces, plus any stock allowance you have defined.
Options Tab
Use the following cutting tool related options on this tab:
Cutting Tool Adapter—Select a part or assembly to use as a cutting tool adapter.
Approach Axis—Select an axis to be used by the tool as an approach to the surface being machined.
First Slice Only—Select this check box to apply the approach motion to the first slice.
Exit Axis—Select an axis to be used by the tool as an exit to the surface being machined.
Last Slice Only—Select this check box to apply the exit motion to the last slice.
Tool Motions Tab
Select options on this tab to create, modify, and delete tool motions and CL commands for defining cut motions.
Alternatively, right-click the graphics window and select Tool Motion Options.
With the Return to Step Options on the shortcut menu in the graphics window you can switch from editing tool motions and editing step references. This option is available only when all references for tool path computation are successfully defined.