Linking Parameters: Thread Mill
Use the Linking Parameters page to define clearance and feed planes for a Thread Mill toolpath.
Absolute and Associative calculations are not available if Output format is set to 4-axis or 5-axis on the Tool Axis Control page.
| 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. |
Calculate incremental values from holes/lines
Calculates the Retract, Feed plane, and Top of stock values from the top of the hole or line. When not selected, Mastercam uses the Retract, Feed plane, and Top of stock values specified in the fields.
Automatic linking
Modifies your Clearance, Retract, Top of stock, and Depth parameters to avoid collisions with the solid model or the selected avoidance geometry. When you select Automatic linking, Mastercam warns you that the settings have been changed.
Arc fit maximum radius
Attempts to fit 90-degree arc moves into rapid and clearance moves. If the entered radius does not fit, then the output is created as an 180-degree arc.
Output feed move
Outputs all rapid moves between passes as a feed rate move instead of a rapid move. This is helpful when the tool needs to make many irregular moves per pass to jump between different areas of the part. This option is also useful for older machines which create dogleg moves for rapids.
| Arc fit maximum radius and Output feed move off | Arc fit maximum radius and Output feed move on |
|---|---|
|
|
Clearance
Sets the height at which the tool moves to and from the part. Select the checkbox to activate the clearance height. If it is not selected, the Retract value is used as the clearance plane. Click the button to set or change the height. You can select a point on the geometry or enter a value.
For Thread Mill toolpaths, Clearance sets the height that tool rapids to before and after cutting each thread. This is an absolute value.
Use clearance only at the start and end of operation
Rapids to the clearance plane only at the start and end of the toolpath.
Retract
Sets the height that the tool moves up to before the next tool pass. Select the checkbox to activate the retract plane, and then click the button and select a point on the geometry or enter a value. The retract height should be set above the feed plane.
For Thread Mill toolpaths, Clearance sets the height that tool rapids to before and after cutting each thread. This is an absolute value.
For Multiaxis toolpaths and Drill toolpaths with multiaxis functionality enabled, Retract is an incremental distance from the current tool position.
For Model Chamfer toolpaths, the incremental value moves away from the current position and it is gouge checked against the selected solid model and the avoidance geometry. If the distance will gouge, Model Chamfer raises the value higher until it clears.
If you do not enter a Clearance height, the tool moves to the retract height between operations.
Feed plane
Sets the height that the tool rapids to before changing to the plunge rate to enter the part. The tool also moves to this height between operations if you do not enter both the Clearance height and the Retract height. Select the checkbox to activate the feed plane, and then click the button and select a point on the geometry or enter a value.
For Multiaxis toolpaths, Feed plane is an incremental distance from the current tool position.
For Model Chamfer toolpaths, Feed plane is an incremental distance above the next cut depth.
Top of thread
Sets the highest height of the toolpath. This can be an absolute or incremental value. Select the checkbox to activate the retract plane, and then click the button and select a point on the geometry or enter a value.
Thread depth
Sets the final machining depth at the bottom of the thread. This can be an absolute or incremental value. Select the checkbox to activate the retract plane, and then click the button and select a point on the geometry or enter a value.
Absolute
Absolute values are always measured from the origin 0,0,0. If you were to translate geometry associated with a toolpath, and the toolpath depth were set to an absolute value, the tool will try to cut to that same absolute depth value no matter where the geometry is located.
Incremental
Incremental values are relative to other parameters or chained geometry.
For most Mill and Router toolpaths, Depth and Top of stock parameters are relative to the location of the chained geometry. Clearance, Retract, and Feed plane are relative to the Top of stock.
For multiaxis toolpaths, all Clearance, Retract, and Feed plane values are an incremental distance from the current tool position.
For 3D high speed toolpaths, the incremental Clearance distance is calculated relative to the adjacent feed-rate move. Note that this option does not result in incremental coordinates being output in the NC program; use the Control Definition Manager to determine that.
Associative
Associative values are measured relative to a selected point on the feature. Use Select point to choose the point from which the associative value will be measured. Use Delete point to remove the associative point.
Calculate depth from top of stock
Enabled when Use Stock is selected on the Stock page. Adjusts the machining depth relative to the top of the stock.
When Use stock is selected on the Stock page, toolpaths are created relative to the stock model. This creates more accurate and efficient toolpaths when using an uneven stock model. When Use stock definition is set to Feed position, Depth, or Both on the Stock page, the corresponding values are locked to Incremental.





