Thread Milling Cycle

Thread milling is a very useful alternative to standard thread cutting (Tap cycle) or thread forming for the production of internal and external threads as it produces threads with excellent form, finish, and dimensional accuracy. During the machining process the tool spirals either up or down around the thread diameter that is specified by the selected curve. It is also very important that the CNC control supports circular interpolation (arc moves) in combination with Z axis movements and the EZCAM postprocessor is set up accordingly.

The EZCAM Thread Milling cycle is designed to machine inside/outside threads with the use of single or multi tip milling tools. This includes left/right-hand threads as well as the choice of selecting the machining direction (upwards/downwards). Accordingly ramp-in/out moves are automatically attached. Cutter compensation can be used on the tool path if Cutter Comp is turned on. An additional contour offset can be defined by using the Stock Allowance setting. The Feedrate Adaption option controls feedrate on all arc moves so that the defined milling feedrate refers to tools outside diameter instead of the tools center line.

To open the thread milling dialog for editing, double-click the desired Work Step in the selection list box. The tool diameter, pitch and depth settings from the thread milling dialog are also found on the Tool Info and Cycle Data tabs of the regular Work Step dialog. They can be edited in both places. The Ramp/Lead parameters located on the Cycle Data tab are disregarded.

Select the desired area in the graphic below or scroll down to view the list of available settings and related explanations.

This list box allows to select single or multi tip tools. If multi tip tool type is selected, the Insert Height setting becomes visible. There you have to specify the height of the tool area that is used for machining. This value is used to determine the number of thread revs that are finished with one complete pass (revolution) around the thread diameter.

Single Tip

Multi Tip: Type 1

Multi Tip: Type 2

The tool diameter specified here is used to calculate the center tool path and to adjust the feedrate when the Feedrate Adaption option is activated. This parameter is also found on the Tool Info tab.

This parameter is only visible when the Tool Type is set to multi tip tools. Internally the height is divided by the pitch setting to determine how many thread revs are finished with one full turn around the thread diameter. If multi tip "Type 1" tools are used only one full revolution will be generated and an error message is displayed if the thread depth exceeds the insert height to avoid tool/part damage. For "Type 2" tools, the number of tips on the insert simply reduces the number of revolutions necessary to complete the thread.

Multi Tip: Type 1	Multi Tip: Type 2

The thread type list box let's you decide wether you want to machine inside or outside threads. For inside threads, the arc radius of the machined curve represents the outside thread radius and the root diameter (D) defines the ramp-in/out radius. When machining outside threads, the root diameter (D) defines the thread radius and the curves arc radius is used for positioning and to calculate the ramp-in/out radius. For all thread types, the tool will always ramp-in/out at the 0° degree position of the thread diameter.

Inside

Outside

The graphic examples above display the center tool path for both thread types. The green circle visible on the inside of the blue curve was only defined to visualize the root diameter specified on the thread milling cycles dialog. See the Root Diameter and Curve Creation Rules topics for more information.

This setting defines the thread's pitch in Threads Per Inch (Tpi) in INCH mode or millimeter per revolution in METRIC mode. See the interactive graphic of the Setup dialog for more information about Inch/Metric settings. This parameter is also found on the Tool Info tab.

This parameter sets the depth of the thread and therefore specifies how far below the Z Surface parameter (or the machining surface) the tool will cut. See the Z Data topic for more information on depth settings. This parameter is also found on the Tool Info tab.

These two settings specify a percentage factor that is applied to the feedrate used to ramp-in/out. If Feedrate Adaption is used, the ramp feedrate calculation is based on the "adapted" feedrate. Otherwise the Feed (XY) setting located on the Tool Info tab of the Work Step Data dialog is used.

This list box provides two options to define the machining direction. If upwards (default) is selected, the tool will first plunge to the final depth of the thread and then begin to spiral out in positive Z axis direction. The resulting tool moves will be counter-clockwise for right-hand and clockwise for left-hand threads. If downwards is selected, the tool will spiral down until the final depth is reached at the end of the ramp-out move. In that case, the tool moves will be clockwise for right-hand and counter-clockwise for left-hand threads.

The table below gives detailed information about the Z axis moving sequence that is resulting from the selected machining direction.

Machining Direction = Upward

Machining Direction = Downward

For inside threads, the arc radius of the machined curve represents the outside thread radius and the root diameter (D) is only used to calculate the ramp-in/out radius. When machining outside threads, the root diameter (D) defines the thread radius and the curves arc radius is used to calculate the ramp-in/out radius.

When milling in a circular path, the outside diameter of the tool is feeding at a rate different than that of the tool's centerline. When feedrate adaption is activated (default), the programmed feedrate (center tool path) on all arc moves is reduced (inside arcs) or increased (outside arcs) in order to maintain the specified Feed (XY) (see Tool Info tab) on the tool's outside diameter. In that case the Ramp-In/Out factors will use the adapted feedrate to calculate the ramp-in/out feedrate.

Inside Thread	Adapted Feedrate = Feed (XY) x ( DThread - DTool ) / DThread
Outside Thread	Adapted Feedrate = ( Feed (XY) x DRoot ) / ( DRoot - DTool )

When this button is selected, all user inputs are checked and the thread milling dialog is closed before opening the Work Step Data dialog.

This button is used to store the current dialog settings as default values for subsequent Work Steps or when restarting the software. It is important to know that the current settings of the Work Step Data dialog are stored too.

This button opens the EZCAM help file, guiding the user directly to the current cycle related help topic.

When this button is selected, all user inputs are checked and the dialog is closed.

This button closes the cycle dialog without accepting any inputs or alterations.

A curve used for thread milling operations consists of at least two connected arc moves that represent the full thread circle. These arc moves are very important since the cycle needs the arc radius for various calculations. The curve direction (clockwise / counter-clockwise) is not important since the machining direction is automatically determined by the thread type, machining direction and thread direction settings. The arc radius also always specifies the outside diameter for inside and outside threads.

Geometry Circles	Chained Curve

Simulated tool path using the Verify command

The easiest way to create such curves is to draw circles at the desired thread location(s). After creating a new curve with the New command from the Curves menu, select the Chain command to chain the circle(s). This will automatically create the two connected arc moves that represent the full circle for the curve. The same command can be used repeatedly to connect subsequent circles to the same curve. Depending on the Rapid Mode toggle, multiple circles are connected with linear or rapid moves.

For more information about chaining circles and graphic examples see the Chain command topic.

There are two settings that actually control cutter compensation and CAM offset. They can be used independently or in combination.

The first is the Cutter Comp list box located on the Tool Info tab of the Work Step dialog. If set to left or right, the software will output the corresponding G-Code (G40/41/42) commands in the machine program. For the thread cycle the direction itself is not important since it is automatically determined according to the thread cycle parameters. The linear approach and retract moves to activate/ deactivate the cutter compensation are generated automatically by the system. Therefore the standard Ramp/Lead parameters located on the Cycle Data tab are disregarded.

Second is the Offset Direction list box located on the Cycle Data tab. If set to left or right, the software will compensate the tool radius and compute the center tool path in the machine program. Therefore this is named CAM offset. As mentioned for the previous Cutter Comp setting, the direction itself is not important and determined automatically.

If you intend to handle the cutter compensation completely on the machine, set the Cutter Comp to Left or Right and Offset Direction to OFF.