When using the Profile Group Parameters dialog for a Turning 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).
Tool Orientation — Select the direction from which the tool cuts (Right or Left).
X-Finish (Fx) — Enter the width of the finishing cut in X.
Z Finish (Fz) — Enter the width of the finishing cut in Z.
Depth of Cut (d) — Enter the amount of material removed on each tool pass.
Return Length (l) — Enter the distance (above the previous cut that was made) at which the tool retracts.
Return Angle (a) — Enter the angle at which the tool retracts to move to the return length.
Diameter Clearance (Cd) — Enter the X distance from the stock that the tool retracts after the initial cutting pass. Also the X distance between the part and the Cutting Point when the cutting point is defined at the stock corner.
Face Clearance (Cf) — Enter the Z distance from the stock that the tool retracts after the initial cutting pass. Also the Z distance between the part and the Cutting Point when the cutting point is defined at the stock corner.
Surface Roughness — Enter the surface roughness of the operation, as measured in µin for inch mode and µm in metric mode.
Operations — Select the type of operations to be performed:
- Roughing — Select the Roughing option to include a roughing pass operation.
- Finishing — Select the Finishing option to include a finishing pass operation.
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.
Leads — Click 
to display the Leads dialog, where you can control the movement of the tool as it:
- Approaches the stock before starting a cutting move (Leads In). Leads In consist of an arc that is tangential to the start of the profile and a line tangential to this arc.
- Leaves the stock at the end of a cutting move (Leads Out). Leads Out consist of an arc that is tangential to the end of the profile and a line tangential to this arc.
PartMaker creates Lead In and Lead Out moves when a profile group is created.
Cutting Point — Click this button to display the Cutting Point dialog, where you can define the Cutting Point for the profile group. The Cutting Point is the point that defines the outside limits of the material to be removed.
Bi-directional Cutting — Select this option to use bi-directional cutting.
Pinch Turning — Select this option to specify that the group supports Pinch Turning (also known as, balance turning). Pinch Turning uses two turning tools, each mounted on a separate tool post. Both tools machine the same part profile simultaneously, where one tool leads while the other follows its path at a specified depth of cut. Pinch Turning helps reduce the cycle time when performing multiple-pass turning operations.
Part Profile — Select the profile shape:
- Open defines a profile that is open on one side.
- Bounded defines a profile that is bounded on both sides.
Toolpath Trimming — Select whether you want to trim the toolpath to a stock profile or not.
Cutting Limits Defined By — Select how you want to define Cutting Limits. Cutting limits define the area in which all cutting moves occur when machining a Turning toolpath.
- Cutting Point — Select this option to define the Cutting Limits using the Cutting Point. This option is available only when None is selected in the Toolpath Trimming list.
- Part Profile Boundaries — Select this option to define the Cutting Limits using the boundary of the part profile. This option is available only when None is selected in the Toolpath Trimming drop-down menu.
- Stock Profile Boundaries — Select this option to define the Cutting Limits using a Stock Profile Boundary. This option is available only when To Stock Profile is selected in the Toolpath Trimming drop-down menu.
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.