When using the Profile Group Parameters dialog for a Thread Mill strategy, the following settings are available:
Thread Type — Select the type of thread to be machined:
- External — Select to cut an OD thread that is on a round extrusion.
- Internal — Select to cut an ID thread that is inside of a hole.
Style — Select the type of style to be used:
- Top Down — Select this option so the tool starts at the clearance position and moves downward in a helix to cut the thread.
- Bottom Up — Select this option so the tool starts at the depth of the thread and moves upward in a helix to cut the thread.
Thread Direction — Select the direction of the thread:
- Right Hand — Select to cut a right-handed thread, which is standard in threading applications.
- Left Hand — Select to cut a left-handed thread.
Z_Surf (S) — Enter the signed distance from the zero reference point to the part surface.
Z_Depth (D) — Enter the depth of the operation to be performed.
Z_Rapid (R) — Enter the distance between the bottom tip of the tool and the part surface when a tool performs rapid moves.
Z_Clear (Cl) — Enter the distance between the bottom tip of the tool and the part surface when a tool starts feeding into the part.
Operations information
- Roughing — PartMaker automatically selects this option to include a roughing pass operation.
- Diam (d) — Enter the diameter of the tool used to perform the operation.
- Tool ID — Enter the ID of the selected tool. When you have saved the group, you can click the icon showing a representation of the tool (for example
) to display the Edit Tool dialog to view, or modify, details of the tool. - Pitch — Enter the distance between the teeth of the thread for the operation. The default value of this option is calculated from the Threads Per Inch value (Inch units) or taken from the Pitch value (metric units) from the tool's properties in the Tool Data dialog.
- 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. The arc move of the Lead In maintains its vertical tangency with the cutting toolpath's helical move (that is, the Lead In arc move will be a helical move).
- 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. The arc move of the Lead Out maintains its vertical tangency with the cutting toolpath's helical move (that is, the Lead Out arc move will be a helical move).
PartMaker creates Lead In and Lead Out moves when a profile group is created.
Lock Toolpath —Select this option to lock the toolpath. When a toolpath is locked, PartMaker does not recalculate it even if its settings on the Profile Group Parameters dialog change. Deselecting this option unlocks the toolpath.
Polar Style Output — Select this option to specify whether the NC program is in polar format. This allows for Posts to explicitly support machining without polar interpolation activated in the NC code.
- When selected, the post will typically output X and Y positions with polar interpolation activated.
- When deselected, the Post will typically output Radius and C-angle positions without polar interpolation. Deselecting Polar Style Output can simplify helical moves at the centerline of the part, or a series of lines that are along a helical path at the centerline of the part, meaning you can have a single ZC line to represent a helix cut the length of the thread rather than a series of arcs.
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.
Thread Mill Options — Click to display the Thread Mill Options dialog, where you can specify additional options when using a Thread Mill cycle.
Extract Parameters From Solid — Select this option to extract geometric information from the imported solid model and use this information to complete some of the fields on this dialog. When you have selected this option, select surfaces on the solid model and then click Extract to extract the geometric information. Press the Shift key to select more than one surface at a time. Click Undo to revert any values on the dialog that have been calculated by extracting geometric data from the solid model back to their original values.