In the following section of the tutorial we will generate a Threading NC program. In order to select the Threading Horizontal operation the below described steps must be performed.
You can watch the related video for this part of the tutorial here:
Creation of Threading Toolpaths
Ensure the file type (NC Format) for our threading example program is ISO Turning.
Then select the feature Threading Horizontal by clicking on the Threading Horizontal icon in the Turning Operations toolbar.
This will open the Threading Z 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 Z: This is the Z value where the operation starts.
End Z: This is the Z value where the operation ends.
Click on the button Parameters in the Threading Z Turning pane to open the parameters dialog. Enter the following values into the parameter dialogs shown below.
Thread Form Tab
Configures the form of the thread in the operation.
Threading Type: The four icons represent threading outside or inside made from left to right, or right to left.
Thread Lead: Defines the starting position of the thread.
Number of Starts: This defines how many starts the thread will have; the normal number is one.
Select From Table: Instead of typing all the various values for the thread, these can be inserted from a table. This table contains all of the most common threads for both Imperial and Metric. Please see the section Select Thread for further explanations on the use of the table.
Included Angle: The total angle of the thread profile.
Thread Angle: The forward angle of the thread profile measured from vertical.
Major Diameter: The largest measure of the thread diameter.
Minor Diameter: The smallest measure of the thread diameter.
Cutting Tab
Configure the number of and the type of cuts that should be used in the operation
Constant Area: Using the constant area option, the tool will remove equal amounts of the area per cut.
Constant Depth: Using the constant depth option, each cut will have the same depth. Since the removed area is triangular an increasing amount will be removed the deeper the tool cuts.
First Cut Depth: If this option is selected, the first cut defines how the following cuts will be made based on what method (Constant Area/Depth) is used.
Number of Cuts: If this option is selected, the operation will be performed with this number of cuts (plus the selected number of spring cuts).
Number of Spring Cuts: If spring cuts are used, this many cuts will be made at the final depth.
Stock Clearance: Defines how far away from the stock the tool should move before it moves back to the start.
Stock to Leave: Defines how much stock should be left at the end of the operation.
Pulloff Distance: Defines the distance (Absolute or in Revolutions) that should be covered at the end of each cut (only used with canned cycles).
Infeed Angle: The angle at which the tool will move down. The reason for this is to minimize the chip pressure at the front of the tool and thereby obtain a more even thread.
NC Export Type: Use this field to select how the thread cycle should be exported.
Taper Tab
Configures extension of the cuts and a possible taper for the operation.
Taper Type: If the taper angle is not zero, a conical thread will be produced. The two icons represent the two ways the cone can go.
Taper Angle: Is the angle of the conical thread.
Absolute (Overcut): With this option the tool will continue the defined distance at the end of the thread.
Revolutions (Overcut): With this option the thread will be extended by the number of revolutions entered.
Acceleration Distance: The Distance that the tool will start before reaching the thread in order to accelerate to achieve a more uniform thread.
Calculation (Acceleration Distance): With this option the acceleration distance will be calculated by the operation.
Absolute (Acceleration Distance): With this option the user can enter how far away the tool should start before reaching the thread.
Revolutions (Acceleration Distance): With this option the tool will use the given number of revolutions to accelerate. It will therefore start the number of revolutions multiplied by the thread pitch before reaching the thread.
Click on OK to use the values and close the dialog.
After the values have been entered in the dialog the screen will look something like the picture below. Notice that the area of operation is shown with a blue rectangle.
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.
icon in the Turning Operations toolbar.
Paste from the Edit toolbar in the Editor tab.
icon in the File toolbar.
