Manufacturing > Milling > Conventional Milling > To Create a 3-, 4-, or 5-Axis Conventional Milling NC Sequence
  
To Create a 3-, 4-, or 5-Axis Conventional Milling NC Sequence
1. Ensure that the active operation references a workcell having milling capability.
2. Click Mill > Milling > Conventional Milling. The Conventional Milling tab opens
 
* You can also create or edit a step from the Process Manager. For details, see To Insert a Milling Step.
3. Depending on the type of workcell the operation references, select one of the following:
◦ —3–axis machining.
◦ — 4–axis machining.
◦ —5–axis machining.
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 all 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 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 or click the again.
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 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.
7. Specify the cut angle in the box adjacent to . The cut angle is relative to X axis of the coordinate system you are using for the milling NC sequence. Alternatively, you can specify the cut angle from the Parameters and Cut Direction tabs.
You can click to flip the cut angle.
8. Select the following options on the Reference tab:
◦ Type—The following types are available:
▪ Surface—This type is selected by default. It includes individual surfaces, quilts, planar surfaces, mill surfaces or datum planes as references.
▪ Mill Window—Select to use a mill window as machining reference.
▪ Previous Step—Select to use previous step as machining reference.
◦ Machining References—Depending on the type of reference you have selected, select the mill window, the previous step, or surfaces as machining references. Alternatively, right-click the graphics window and select Machining References from the shortcut menu.
◦ Loops To Close—Specify loops to close if you select Mill window for machining. Alternatively, right-click the graphics window and select Closed Loops from the shortcut menu. This option is available for the Mill window type.
◦ Scallop Surfaces—Select surfaces to be excluded from scallop computation. Alternatively, right-click the graphics window and select Scallop Surfaces from the shortcut menu.
9. 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 Conventional milling.
Alternatively, right-click the graphics window and select Parameters from the shortcut menu.
10. On the Clearance tab, optionally specify the following:
◦ Retract—Specify the Reference 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.
11. On the Cut Direction tab, click one of the following options:
◦ Angle—Specify the cut angle. The direction of the cuts is defined by an angle from the x-axis of the NC Sequence coordinate system. Alternatively, you can specify the cut angle in the box adjacent to Angle.
◦ Reference—Select a straight edge or a datum plane as a reference for cut direction.
Click Scan Preview to preview the surfaces of the reference part from where the tool will move or scan while machining.
12. Use options on the Check Surfaces tab to 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 Options tab, open a part or assembly to use as a cutting tool adapter. Alternatively, click to copy cutting tool adapter from another step.
14. On the Tool Motions tab, select the options 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.
 
* With the Return to Step Options option 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.
15. Click to get a dynamic preview of the tool path in the graphics window.
16. 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.
 
* The Prerequisites option is available on the Process tab while creating or editing a step from the Process Manager.
17. 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.
18. 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.
19. 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.
◦ Click to cancel the changes.