In the following section of the tutorial we will generate a Drilling NC program. In order to select the Drilling operation the below described steps must be performed.
You can watch the related video for this part of the tutorial here:
Generate a Drill Cycle
Ensure the file type (NC Format) for our drilling example program is ISO Turning.
Then select the feature Drilling by clicking on the End Drilling icon in the Turning Operations toolbar.
This will open the End Drilling pane to the left of the drawing area. Now insert the values shown in the dialog below.
Comment: This comment will be shown in the final NC Program. It is always good to include a comment in order to distinguish the various operations in the final program.
Retract Distance (Abs.): The distance to which the tool is retracted after the operation has been completed.
Safe Distance (Abs.): The distance from the start of the operation where the feedrate will switch from rapid to feed.
Start Depth: The depth at which the actual operation is started.
End Depth: The final depth of the operation.
The Drilling operation is defined by the above parameters, after the entry of which the screen will look something like the one shown below.
The four distances entered are shown as crosses on the drawing.
Click on the button Parameters in the End Drilling pane to open the parameters dialog. Enter the following values into the parameter dialogs shown below.
Drilling Parameters
Operation Type: The operation type can be Drilling G83 or Tapping CW G84 for Canned cycles, and Drilling or Peck drilling for Longhand cycles.
Use Upper Dwelling: Toggles the use of upper dwelling. Upper Dwelling is the time that the drill will rest at the top of a peck.
Use Lower Dwelling: Toggles the use of lower dwelling. Lower Dwelling is the time that the tool will rest at the bottom of each cut in order to break the chip.
Use Plunging Feedrate: Toggles the use of Plunging Feedrate. This is the feedrate used during the drilling part of the operation.
Use Retract Feedrate: Toggles the use of Retract Feedrate. This is the feedrate used during the retract part of the operation.
Use Tip Compensation: Toggles the use of tip compensation. This option is used for drilling through a part. It will extend the hole based on the geometry of the drill.
Tip Angle: The angle of the drill.
Drill Diameter: The diameter of the drill.
Tip Compensation: The length of the tip of the drill. This is the length from the tip to where the drill reaches the full diameter.
Use Pecking: By selecting this option the operation will be performed with pecking movements.
Peck Clearance: The distance away from the current bottom of the hole where the feedrate will switch from rapid to feed.
Peck Retract: The distance that the tool will retract between pecks (must be larger than Peck Clearance).
First Peck: The distance that the tool moves down in the first peck. This is the depth of the first peck.
Subsequent Pecks: After the first peck is performed, the entered distance will be used for the remaining pecks.
The selected operation type determines which drill parameters are available.
Click on OK to use the values and close the dialog.
Try experimenting with the various parameters and see how they change the generated toolpath.
Exporting the Toolpath and Backplot in the Editor
Click on Export Clipboard in order to generate the actual program. The program is now in the computer's clipboard and is ready to be inserted into the CNC program.
Change the window to the NC program and move the cursor to the very end by pressing Ctrl+End. Insert the text from the clipboard, either by pressing Ctrl+V, or selecting the icon Paste from the Edit toolbar in the Editor tab.
Now the NC program should look like the following screen.
To verify the generated toolpath, we must simulate it using the integrated Graphical Backplot.
To open the backplot window, click on the Backplot tab at the top of the Ribbon and then on the Backplot Window icon in the File toolbar.