When using the Profile Group Parameters dialog for a Threading turn strategy, the following settings are available:
Strategy — Select the type of strategy to be performed.
Tool Location — Select the location of the tool (In, Out or Face).
Toolpath Options — Select one of the following options:
- Chamfer on Exit — Select to include a chamfer on exit, so the threaded profile is bounded.
- No Chamfer — Select so no chamfer is included, and the threaded profile is unbounded.
Tool Orientation — Select the direction from which the tool cuts (Right or Left).
First Infeed (i) — Enter the depth of material removed in the first axial pass.
Minimal Infeed (j) — Enter the depth of material removed in subsequent axial passes.
Thread Height (H) — Enter the height of the threads. This can be defined as a percentage of a pitch or as a direct measurement in part units, depending on the method selected in the Defaults for Turningdialog.
Pitch (p) — Enter the distance between each thread.
Infeed Angle (a) — Enter the angle at which infeed occurs.
Clearance (C) — Enter the X distance from the part along which the tool returns after each pass.
Acceleration Dist (L1) — Enter the distance from the stock at which the tool needs to accelerate to the speed needed to cut the part.
Chamfer Length (L2) — Enter the distance in the Z axis from the end of the last thread to the exit point.
Chamfer Angle (b) — Enter the angle of the chamfer after the last thread in closed stock.
Operations — Select the type of operations to be performed:
- Roughing — This option is automatically selected for profile groups where the Threading strategy is selected.
Tool ID — Enter the ID of the tool you want to use for the selected operation or click Select Tools to choose a tool from the Select Tool dialog.
When a tool has been selected, you can click the icon that shows a representation of the tool to display the Edit Tool dialog, where you can view, or modify, details of the tool.
Thread Options — Click to display the Thread Options dialog, where you can enter additional settings for threading cycles.
Group Name — Enter a name for the profile group.
Select Tools — Click to display the Select Tool dialog, where you can select the tool to use for machining.