Manufacturing > Manufacturing > Milling > Thread Milling > To Create a Thread Milling NC Sequence
To Create a Thread Milling NC Sequence
1. Ensure that the active operation references a Mill or Mill/Turn workcell.
2. On the Mill tab, click the arrow next to the Milling group.
3. Click Thread Milling. The Thread Milling 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. Select to create internal threads or select to create external threads.
9. Select any one of the following thread cut type:
—Cuts a straight thread. This is the default thread cut type.
—Cuts a pipe taper thread, which has a nominal angle of 1.7899 degrees. This value is preset by Creo NC.
For pipe tapered threads, the THREAD_DIAMETER parameter is achieved at the last GOTO point in the cut. This is represented by the Start reference in a hole set for an internal thread, and the End reference in a hole set for an external thread.
—Cuts a taper thread with a custom taper angle specified using the TAPER_ANGLE parameter.
10. On the References tab, select the following options. You can cut threads on features such as holes bosses, and axes.
Threads—Select the features to be threaded . The number of selected features is displayed in the collector. The selected features form the first thread set, which is displayed as Set 1. To create another set of holes for threading, click New set and select the holes to form Set 2.
Alternatively, right-click the graphics window and select Add Thread Set from the shortcut menu.
Click Details to open the Thread Set dialog box. Select the features to be included in a thread set using various selection methods.
Select options from the Start and End list to set the initial and final depth and to specify the start and end surfaces for thread milling. For details, see The Thread Set Dialog Box in Related Links.
11. 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 thread 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.
12. 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.
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 Definition 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 trajectory 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.