In the following section of the tutorial we will generate a Finish NC program. In order to select the Finish operation the below described steps must be performed.
You can watch the related video for this part of the tutorial here:
Creation of Finishing Toolpaths
Ensure the file type (NC Format) for our finishing example program is ISO Turning.
Then select the feature Finish Turning by clicking on the Finish Turning icon in the Turning Operations toolbar.
This will open the Finish Turning 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 Point Z: This is the Z value to where the operation will retract the tool after completion.
Retract Point X: This is the X value to where the operation will retract the tool after completion.
Radial Min: This is the lower machining limit for the operation in the X direction.
Radial Max: This is the upper machining limit for the operation in the X direction.
Use Axial Stock Limits: This option indicates if axial limitis should be used.
Axial Min: This is the leftmost machining limit for the operation in the Z direction.
Axial Max: This is the rightmost machining limit for the operation in the Z direction.
The Finish operation works on a contour, and in order to generate a toolpath we must select that contour. To select the contour for the operation perform the following steps:
Ensure that Single Step is unchecked in the Finish Turning pane.
Select the contour shown on the picture below. To do this, start at the far right by selecting the vertical line with the indication arrow pointing up. Now the whole contour is selected, so unselect the last vertical line by clicking the Back button.
Now your drawing should look something like the one below.
Click on the button Parameters in the Finish Turning pane to open the parameters dialog. Enter the following values into the parameter dialogs shown below.
Tool Tab
Configures settings for tool, work orientation and compensation type used for the operation.
Tool Orientation: The nine icons represent the possible nine orientations of the tool.
Tool Radius: The nose radius of the tool.
Work Orientation: The four icons control the way we machine the part. In the following we are machining outside from right to left.
Use Axial Plunge: If the tool permits it, check this option to allow horizontal plunge.
Use Radial Plunge: If the tool permits it, check this option to allow vertical plunge.
Plunge Angle: Is the maximum angle we will allow the tool plunge.
Compensation Type: This is the compensation type that is used for the operation. The two most commonly used are Controller or Computer.
Cuts Tab
Configures cutting parameters for the operation.
Passes: The number of finish passes to take in the operation.
Spacing: The depth of each of the finish passes.
Retract Distance: The distance that the tool retracts from the stock before a return move is made.
Stock to Leave X: Is the amount of material that will be left in the X-direction after the whole operation is performed.
Stock to Leave Z: Is the amount of material that will be left in the Z-direction after the whole operation is performed.
Entry/Exit Tab
Configure how the tool approaches and leaves the part.
Entry Amount: This value is used to extend the toolpath before it starts the actual cut.
Extension: This values is used to extend the toolpath at the end of the cut.
Use Entry Vector: Enable/Disable the use of entry vector.
Entry Angle: The angle at which the tool will approach the part.
Entry Length: The length of the approach.
Use Exit Vector: Enable/Disable the use of exit vector.
Exit Angle: The angle at which the tool will retract from the part.
Exit Length: The length of the retract.
After entering the values, close the parameters dialog with OK. To show the generated toolpath on the drawing click on Show Toolpath button in the Finish Turning pane.
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.