Cut Parameters: Thread Mill
Use the Cut Parameters page to enter cutting parameters and compensation options for your Thread Mill toolpath.
| Icon | Name | Description |
|---|---|---|
|
Detect (FBM Drill) | Analyzes the solid model and detects features based on the Feature Based Machining (FBM) operation's current parameters. View the results of all detected features and their machining information in the Features page. For more information, please refer to Detection States and Modes in FBM. |
|
Reselection is not available | Hole Wizard features for a Wizard Holes operation can only be selected in Mastercam for SOLIDWORKS. Contact your Reseller for more information. |
|
Preview toolpath operations (FBM Drill/Wizard Holes) | Opens the Toolpath Operations Preview dialog box where you can view the list of operations FBM will generate using the current Features page list. |
|
Save parameters to defaults file | Makes the current toolpath settings the default for future toolpaths of this type. Saves the current values in the toolpath properties pages to the .mcam-defaults file specified in the machine group properties. |
|
Reload parameters from defaults file | Overwrites the current values in the toolpath properties pages with the toolpath's default parameters. These parameters are reloaded from the .mcam-defaults file specified in the machine group properties. |
|
Hide dialog | Minimizes the dialog box so that you can use other Mastercam functions, like changing your shading settings or the graphics window view. When finished, press [Esc] to maximize the dialog box. |
|
Tool Manager | Opens the Tool Manager. Use the Tool Manager to create and edit tool definitions and to work with tool libraries. When you close the Tool Manager, the toolpath dialog box will reappear just as you left it. |
|
Feed speed calculator | Opens the Feed & Speed Calculator dialog box where you can modify the calculated feed rate or spindle speed by adjusting the material and tool parameters. |
|
None |
Page window | This window displays all of the pages that are available to you, depending on the selected toolpath type. A green check mark indicates pages where data has changed in the current session. |
| None | Quick View Settings | This window summarizes key toolpath information from the Tool page, Coolant page, and Planes page. It updates automatically as you make changes to the different pages and is always visible. |
| None | Generate toolpath | When selected, automatically generates the toolpath when you click OK. For more information, refer to Accepting and Generating Toolpaths. |
|
OK | Generates the toolpath and closes the dialog box. If editing a toolpath, applies the changes and closes the dialog box. |
|
Apply | Applies your changes to the toolpath without closing the dialog box. |
|
Cancel | Closes the dialog box and cancels the toolpath creation. If editing a toolpath, any changes to the toolpath are discarded. |
Number of active teeth
Sets the number of teeth used to cut the thread. You can enter a value of 1 even for multi-tooth cutters. A greater number of active teeth reduces the number of revolutions needed to cut the thread.
Lock
Locks the value of the corresponding parameter. Mastercam will no longer recalculate the value when changes are made to the Tool page and you cannot edit the value until the parameter is unlocked.
Thread pitch
Sets the distance between the teeth of the thread mill tool.
Lock
Locks the value of the corresponding parameter. Mastercam will no longer recalculate the value when changes are made to the Tool page and you cannot edit the value until the parameter is unlocked.
Thread start angle
Defines the angle at which the start of the thread is cut after the entry arc is machined. If the thread is machined from top to bottom, the angle applies to the top of the thread. If the thread is machined from bottom to top, this angle applies to the bottom of the thread.
Allowance (overcut)
Increases the thread diameter for ID threads. Reduces the thread diameter for OD threads.
Taper angle
Specifies the thread taper angle (usually for pipe threads).
Compensation type
Choose how you want to handle cutter compensation:
- Computer: Computes the compensated toolpath and does not output control codes for compensation.
- Control: Outputs control codes for compensation and does not compute the compensated toolpath.
- Wear: Computes the compensated toolpath and outputs control codes for compensation. Compensation direction in the computer and control are the same.
- Reverse wear: Computes the compensated toolpath and outputs control codes for compensation. Compensation direction in the computer and control are opposite.
- Off: Programs the tool tip directly on the chained geometry and does not output compensation codes.
The available options are determined by the active control definition.
ID thread
Creates an inside diameter (ID) thread.
OD thread
Creates an outside diameter (OD) thread.
Override geometry diameter
Only enabled when arcs, solid arcs, or cylindrical features are selected. Overrides all of the selected geometry's diameter information and forces the output to the specified Major/Minor thread diameter.
Major/Minor thread diameter (Override geometry diameter)
Enabled when Override geometry diameter is selected.
- If you are creating an ID thread, enter the major diameter in this field. This is the diameter at the outermost point of the toolpath.
- If you are creating an OD thread, enter the minor diameter in this field. This is the diameter at the innermost point of the toolpath.
Override minor diameter
Only enabled when arcs, solid arcs, or cylindrical features are selected. Overrides all of the select geometry's minor diameter information and forces the output to the specified Minor thread diameter.
Minor thread diameter (Override minor diameter)
Enabled when Override minor diameter is selected. This is the diameter at the innermost point of the tool. The Minor thread diameter field is used only for collision detection and does not alter the toolpath motion. When you use a threadmill tool, the field is populated from the tool information. If any other tool type is selected, the field shows 0.0. In either case, it can be manually overridden.
Override geometry diameter and Override minor diameter are only available if you select a point entity as the location of
the toolpath, not an arc. If you selected an arc, Mastercam calculates
the proper diameter value.
Right-hand thread
Creates a right-hand thread. Also updates the Climb milling/Conventional milling setting shown in the Machining direction group of the Cut Parameters page.
Left-hand thread
Creates a left-hand thread. Also updates the Climb milling/Conventional milling setting shown in the Machining direction group of the Cut Parameters page.
Top to bottom
Machines the thread from the top to the bottom. Also updates the Climb milling/Conventional milling setting shown in the Machining direction group of the Cut Parameters page.
Bottom to top
Machines the thread from the bottom to the top. Also updates the Climb milling/Conventional milling setting shown in the Machining direction group of the Cut Parameters page.





