Manufacturing > Manufacturing > Milling > Cutline Milling > To Create a 3-, 4-, or 5-Axis Cut Line Milling NC Sequence
To Create a 3-, 4-, or 5-Axis Cut Line Milling NC Sequence
1. Ensure that the active operation references a workcell having milling capability.
2. Click Mill > Milling > Cut Line Milling. The Cut Line 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 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. Select the following options on the References tab:
Type—The option Previous Step is selected by default and the previously created cutline step is added to the Machining References collector automatically before entering the Cut Line Milling tab. To specify machining surfaces, select the Surface option in the list.
Machining References—Select the surfaces to be machined as references. The cut lines that are being defined in the Cut Lines tab depend on these selected surfaces if no alternate surfaces are defined.
Alternatively, right-click the graphics window and select Machining References 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 cut line 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.
9. 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.
10. On the Cut Lines tab, select cut lines to mill the selected surfaces using the following options:
Cut Lines—Select Cutline 1 and Cutline 2 to define cut lines by selecting edges or datum curves and by sketching the cut lines and projecting on the surfaces to be machined. You can machine an open or closed loop of cut lines by appropriately selecting cut lines. The type of the selected reference is displayed in the References collector. To define additional cut lines, select New Cutline. To reorder cut lines and machine them in the selected order, select a cut line name in the list box and click the up or down arrows adjacent to the list box. See topic About Surface Milling for details on cut lines.
Auto Cutline—Select this option to automatically create cut line tool paths for machine references that include a single, closed boundary edge. The boundary edge is automatically selected as the Outer Cutline. The Inner Cutline is a point that you can drag to the desired location.
This option is applicable only for a single machine surface without holes.
Tool Center Curve—Select this option to generate a surface feature representing the zone of the selected surfaces that can be machined using the current tool and parameters. You can then define the cut lines using the edges of this surface. The surface belongs to the NC sequence.
Alternate Surfaces—Select surfaces, other than surfaces to be machined, to be used for defining the cut lines. After you select the entities to define the cut lines from these alternate surfaces, these entities are projected in the direction normal to the alternate surface on the surfaces to be machined to form the cut lines.
Synchronize—Click to open the Synchronize dialog box.
Select Along Cut Line to specify synch points on the cut lines. The cut lines are listed in the Synchronizers box. In the Synchronization Points box, specify the placement of the point as a length ratio along the selected cut line. The system creates the synch line by connecting the synch points with straight linear segments. Click New Synchronizer to add additional synch points along the cut line.
Select Reference Chain and click in the Synchronizer References collector to specify edges of the machining reference as synch points. You can select individual edges, tangent chains, boundary chains, or intent chains. The selected reference chain is added to the Synchronizers box.
Alternatively, right-click the graphics window and select Cut Line References, Cut Line Options - New Synchronizer and Alternate Surface Collector from the shortcut menu.
11. 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.
12. 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.
13. 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.
14. Click to get a dynamic preview of the tool path in the graphics window.
15. 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.
16. 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.
17. 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.
18. 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.