Manufacturing > Manufacturing > Holemaking > To Create a Holemaking NC Sequence
To Create a Holemaking NC Sequence
1. Ensure that you are in a Lathe, Mill, or Mill/Turn work center.
2. Click any one button for the holemaking cycle on the Mill orTurn tab. The tab for the selected holemaking type opens. For example to create standard drilling sequence, click Standard. The Drilling tab opens.
Drilling, Boring, Reaming, Web, Countersink, Face, Tapping, and Custom holemaking types are available. See the topic Holemaking Cycle Types and Tabs for a list of holemaking types available.
Carry out the following steps using the generic options available on a holemaking tab.
3. To switch between any holemaking cycle type, select a cycle on the Model Tree and click Mill > Holemaking Cycles > Switch Cycle or click Turn > Holemaking Cycles > Switch Cycle. Select a cycle type. For details, see To Switch Cycles in Holemaking.
4. 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.
5. Select , , , or to use Head 1, Head 2, Head 3, or Head 4 in the Holemaking sequence.
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.
6. If you have defined a 5–Axes milling work center, or 5–Axes Mill/Turn work center with milling on one or both heads, the option for selecting the number of axes is available. Select for 3–Axis machining and for 5–Axis machining.
7. To preview the cutting tool and its orientation in the graphics window, click adjacent 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.
8. 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 options:
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.
9. Select the following options on the References tab:
Type—Choose one of the following methods for selecting holes to be included in a hole set.
Axes—Holes are represented by datum axes or hole axes. Select individual hole axes to add holes to the hole set.
Points—Holes are represented by datum points. Select individual datum points to add holes to the hole set.
Geometry—Holes are represented by cylindrical surfaces. Select geometry to add holes to the hole set.
Holes—Select the holes to drill by defining hole sets. The number of selected holes are displayed in the collector. The selected holes form the first hole set Set 1. To create another set of holes to drill, click New set and select the holes to form Set 2.
Alternatively, right-click the graphics window and select Add Hole Set from the shortcut menu.
Click Details to open the Holes dialog box to define additional features for holes. For details, see Related Links.
Select manual or automatic from the Start and End lists to specify depth. For manual definition, a collector becomes active to select to select the start and end references for the cycle. For details, see the topic To Define Depth in Related Links.
10. 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 holemaking. 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.
11. 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.
12. On the Check Surfaces tab, define the parts and surfaces that can be used as a limit on the tool motions during machining.
Use this option if there are obstacles (protrusions) along the traversal path between the holes. When the tool traverses from hole to hole and a motion will result in gouging a surface selected as a check surface, the system will issue the CYCLE / OFF command after machining the previous hole, the tool will retract along Z axis to the height of CHK_SRF_STOCK_ALLOW above the obstacle height, and move at FREE_FEED in XY-plane to the location above the next hole, then reissue the CYCLE / ... statement. This functionality is available for all 3-Axis Holemaking NC sequences except Back boring.
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. 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 Definition option on the shortcut menu in the graphics window enables you to 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 roughing 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 animate the tool path display, 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.