Thread Mill Operation dialog - General tab

Compensation - Choose between the Pathtrace and Controller tool radius compensation methods. This determines how the code generator produces CNC code from this command. As a tool radius compensation facility is also present in many CNC control systems, you may wish to consider how best to use these apparently similar facilities.

Mill Type - Select either Climb or Conventional milling. This affects the direction of thread for the cycle.

Canned Cycle - Check for output to be in 3D arc moves. Leave empty for the output to be in linear feed moves.

Tolerance - Specifies the maximum deviation from the thread form when the Code Generator outputs linear feed moves as the cutter path.

Depth

Clearance - Specifies the clearance plane height for the cycle. This is an absolute value.

Retract - Specifies the height the tool retracts to during the cycle. This is a value measured relative to the start height of the thread. In the first link move, the tool rapids to this height and then feeds to the start height.

Upper Distance - Specifies the upper limit of the thread. This is an absolute value denoting the level at which the tool rapids across at in the first link move. Otherwise, digitise an entity from which to take the limit for the thread.

Lower Distance - Specifies the lower limit of the thread. Otherwise, digitise an entity from which to take the limit for the thread.

Thread

Major/Minor Diameter - Normally, you would start defining the thread by selecting an arc entity. This arc represents the major diameter of an external thread, or the minor diameter of an internal thread. You can also digitise a point that represents the centre of the thread (when using the thread milling cycle with hole features for example). In this case, use these fields to specify the major/minor diameter for the thread.

When working with SolidWorks 2001 Plus you can import threading data from SolidWorks into the EdgeCAM Hole Feature dialog. Threading data will be taken from the Tap tab of the Hole Definition in SolidWorks and transferred to the appropriate fields of the Hole Feature dialog. This allows you to set all relevant attributes ready for the application of the operation. The feature attributes Drill Size and Tap Diameter will be taken through to the Major//Minor Diameter fields. Please note that thread details are only passed to EdgeCAM when the EdgeCAM session is started via the launch button in SolidWorks 2001 Plus, and the Thread Information option has been checked on the Feature Finder dialog.

Thread Side - Selects an Internal or External thread.

Hand of Thread - Selects a Right or Left-Handed thread.

Pitch of Thread - Specifies the pitch of the thread (the pitch is the distance travelled down the axis of the thread when the thread has rotated through 360°). Pitch is NOT the same as the lead of the thread, which is calculated as follows:

Lead = Pitch of thread x Number of starts.

Number of Starts - Specifies the number of starts for the thread. If you want more than one start, the starts will be equally spaced around the top of the thread.

Start Angle - Specifies the start angle of the initial thread. The default is 0°. The angle is measured from the direction of the X axis anticlockwise in the direction of the Y axis.

Depth of Thread - Specifies the depth of the thread to be machined.

Cutting Feed - Specifies the feed rate of the actual cutting portion of the cycle.

Speed - Specifies the tool spindle speed in RPM.