Manufacturing > Milling > Trajectory Milling > To Create a 2-Axis Trajectory Milling NC Sequence
  
To Create a 2-Axis Trajectory Milling NC Sequence
In 2-axis Trajectory milling, you define the tool trajectory by sketching or selecting a curve or selecting a model edge that represents the final trajectory of the tool. The curve or edge must lie in the plane normal to the z-axis of the NC sequence coordinate system. In the simplest case, the tool makes just the one cutting pass along this trajectory, with or without tool offset. You can adjust the depth of the final pass, specify multiple cutting passes with a vertical offset, as well as create multiple trajectory milling slices with horizontal offset with respect to the final tool trajectory.
1. Ensure that the active operation references a Mill or Mill/Turn workcell..
2. Click the Mill tab and the arrow next to Trajectory Milling.
3. Select 2 Axis Trajectory. The Curve Trajectory tab opens.
 
* You can also create or edit a step from the Process Manager. For details, see To Insert a Milling Step.
4. Select , , , or for milling 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.
5. 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.
6. 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
7. 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.
8. On the References tab, select the following options :
Machining Reference—Select a curve that lies in a plane normal to the z-axis of the NC sequence coordinate system or select a model edge. You can also asynchronously sketch a curve at this point and select it for the sequence trajectory. A yellow arrow indicates the direction of the trajectory in the graphics window.
Click Details to select related edges or curves and to place them into a group or chain. See topics About Chains and To Trim or Extend a Chain for more information.
Alternatively, right-click the graphics window and select Trajectory Curve to activate the Machining Reference collector.
For more information on selecting loops on surfaces, see topic To Select Loop On Surfaces in 2-Axis Trajectory Milling.
Start Point—Click to open the Start Point dialog box with which you can place the start point of trajectory milling along a curve or an edge segment instead of a vertex. For details see Start Point for Closed Loops in Trajectory Milling.
 
* The Start Point option is not available for machining references with loops on surfaces.
Offset Cut—Select this check box to specify an offset for the cut motion. The offset distance is half of the CUTTER_DIAM value.
Material To Remove—Click to flip the material removal from one side of the reference curve or sketch to the other. The flip direction appears as a purple arrow in the graphics window displaying the material removal side.
You can also right-click this flip direction arrow in the graphics window and change the direction of material removal. This arrow also controls the direction of the tool offset that is set using the Offset Cut option.
Start Height—Select the height from which you want the tool tip to start. The start height is considered only when the value of LAST_FINPASS_OFFSET parameter is greater than 1.
Alternatively, right-click the graphics window and select Start Height.
Height—Adjust the depth of the final pass of the tool by selecting a plane.
Alternatively, right-click the graphics window and select Height.
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 trajectory 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.
10. 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.
11. 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.
12. 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.
13. Click to get a dynamic preview of the tool path in the graphics window.
14. 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 trajectory milling step. Click OK.
 
* The Prerequisites option is available on the Process tab while creating or editing a step from the Process Manager.
15. 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.
16. 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.
17. 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.
 
If you define the finish pass and specify the start height, Creo NC uses the finish pass step depth to compute the number of passes for the NC sequence.
If you define the first pass and specify the start height, Creo NC uses the first pass step depth to compute the number of passes for the NC sequence.
If you define the finish and first pass and specify the start height, Creo NC ignores the first pass and uses the finish pass step depth to compute the number of passes for the NC sequence.