Entry Motion: Dynamic Mill
Use this page to configure an entry method for the Dynamic Mill toolpath. This determines how and where the tool enters the part, and the cutting method/machining strategy used by the toolpath. Other parameters let you further refine the entry moves, and set entry feeds and speeds.
- If you edit the Entry method options, they will not be updated if you re-chain.
- If you select an Entry chain:
- If you select a point chain, Entry method is automatically set to Helix only and Center helix on point is selected.
- If you select a closed/open chain, Entry method is set to Custom, use entry chain.
- If you select a closed/open chain and a point, Entry method is set to Custom, use entry chain.
| 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. |
Entry method
Defines the entry point and cutting strategy used to create the toolpath. Choose one of the following options:
- Helix only: The tool helixes into the pocket and the dynamic pocketing cutting starts right away. This cutting strategy uses a dynamic milling motion growing outward from the entry motion. The helix is centered on the deepest point in the pocket, unless overridden.
- Helix followed by full medial burial: After the helix entry, the tool is fully buried as it moves along the medial axis (central spine of the pocket). Its purpose is to clear a slot for the subsequent passes so that they are not fully buried.
- Helix followed by trochoid medial: The tool enters the pocket with a helix, and then moves along the medial axis (central spine of the pocket) with a trochoidal cut rather than a fully buried cut. This clears a slightly wider slot than full medial burial for the subsequent passes to be optimally engaged. This strategy avoids burying the cutter but takes longer.
- Profile: Creates a “follow boundary” ramp entry based on the shape of the offset pocket. The slot is cleared by taking lighter cuts in the Z axis. Subsequent cuts are properly engaged at the full cut depth.
- Custom, use entry chain: Uses an open chain to define the entry ramp. If an open chain was not previously selected, use the Chain geometry options to add it. The chain must be open, with a start/end gap greater than the chaining tolerance. When using this method, Mastercam requires an open chain to successfully generate the toolpath.
- Plunge only: Plunges directly into the material.
Select
Returns you to the graphics window to select a geometry chain.
Deselect all geometry
Removes all the selected geometry chains from the toolpath. Choose Select (arrow) to return to the Chain Manager where you can add geometry chains for the toolpath.
Helix radius
Available only for helical entry methods. Enter the radius of the entry helix. If the profile is too small for a helix ramp of this diameter, Mastercam creates a profile ramp instead.
Trochoidal loop radius
Only available for Helix followed by trochoid medial. Defines the radius for the toolpath’s trochoidal cut along the medial axis. Enter the radius as an absolute distance.
Additional slot width
Center helix on point
When selected, Mastercam finds the first chained point and centers the entry helix on that point; that is, if it can safely do so without gouging or collision. Otherwise, it positions the entry helix as closely as possible to that point.
Z clearance
Sets extra height to be used in the ramping motion down from a top profile. It ensures that the tool has fully slowed down from rapid speeds before touching the material, so that it enters the material smoothly at the plunge angle.
Plunge angle
Sets the angle of descent for the entry move, and determines the pitch. A smaller plunge angle means that the entry move takes longer to descend in the Z axis. A recommended angle is 3 to 5 percent.
Entry pitch
Controls the entry descent by the pitch value you define. Mastercam descends the tool by the pitch value for every complete revolution of the entry motion, ensuring the tool is never buried by more than the specified pitch.
Skip pockets
Enables the skip pocket parameters. This is useful when the pocket is large enough to accommodate the tool, but the entry move is so compressed that the tool is effectively plunging into the part when Mastercam attempts to machine it.
- Skip all: Skips all pockets.
- Smaller than: Specifies a minimum pocket size for creating
cutting pass. While you can set these values to 0 to ensure that entire surface will be machined, a low value on a cutting area that is too small will result in the tool plunging straight down in the pocket. A more typical value to use is 110% of the tool diameter.
- Tool diameter percentage: Enter a minimum pocket size, as a percentage of the tool diameter. The right field updates to display this value as the minimum pocket size.
Minimum pocket size: Enter a minimum pocket size to create cutting passes. The left field updates to display this value as the tool diameter percentage.
Entry feeds/speeds
Activates the fields in this section for the toolpath. Use the fields to configure an entry ramp feed rate and spindle speed. You can also choose to add a dwell (in seconds) after the entry move before starting the cutting pass. If this option is deselected, Mastercam uses the Feed rate set on the Tools page.
Ramp feed rate
Overrides the feed rate set on the Tools page, and uses the specified feed rate for entry ramps into the cut.
Ramp spindle speed
Overrides the spindle speed set in the Tools page, and uses the specified spindle speed for entry ramps into the cut.
Dwell before cut spindle speed
Adds a dwell (in seconds) after the entry ramp into the cut. This pause allows the spindle time to attain the desired speed before starting the cutting pass.





