Facing the Front of the Stock

In the following section of the tutorial we will generate an NC program to face the front of the part. In order to select the facing operation the below described steps must be performed.

You can watch the related video for this part of the tutorial here:

Creation of Facing Toolpaths

Ensure the file type (NC Format) for our facing example program is ISO Turning.

Then select the feature Face Turning by clicking on the Face Turning icon in the Turning Operations toolbar.

This will open the Face 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.
Start Point Z: This is where the facing operation will start along the Z-axis.
Start Point X: This is the start diameter of the facing operation.
End Point Z: This is where the facing operation will end along the Z-Axis.
End Point X: This is the end diameter of the facing operation.

Now we have defined where the facing operation will work on the stock. This will be shown on the drawing as a rectangle with arrows that indicate the direction of the operation.

Click the button Parameters in the CNC-Calc pane to define how the operation will be performed. Enter the following values into the parameter dialogs shown below.

Cuts Tab

Configures the tool setup and other parameters for the operation.

Tool Orientation: The nine icons represent the possible nine orientations of the tool.

Tool Radius: This is the nose radius of the tool.

Overcut Amount: The distance the tool will cut longer than the End Point X value.

Roughing: Here, the check-box can be used to enable or disable the use of roughing passes. If roughing is used, each cut will be the size of the Roughing Stepover.

Finish: The check box can be used to enable or disable the use of finish passes. If finish passes are used, Finish Cuts passes will be made with a depth of the Finish Stepover.

Stock to Leave: The stock to leave is the amount of material that will be left after the whole operation is performed.

Compensation Type: The compensation type that is used for the operation. The two most commonly used are Controller or Computer.

Entry/Exit Tab

Configure how the tool approaches and leave the part.

Entry Amount: The length that the tool will start each cut above Start Point X.

Retract Amount: The length that the tool will pull free along the Z-Axis before it makes moves for the next cut.

Use Entry Vector: Enable/Disable the use of entry vector.

Entry Angle: The angle of the entry vector.

Entry Length: The length of the entry vector.

Use Exit Vector: Enable/Disable the use of exit vector.

Exit Angle: The angle of the exit vector.

Exit Length: The length of the exit vector.

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 Face 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 Editor in order to generate the actual program. Now, a window like the one shown below will appear. Notice that the comment from the dialog is inserted at the top of the program as a comment.

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.

Now a window like the one below will appear.

The Backplot animation is controlled using the slider and command buttons located in the bottom right.