Entry Motion: Area Mill
Use the Entry Motion page to configure the entry move that the tool will make as it transitions to new Z levels for an Area Mill toolpath. You can choose to create either a ramp entry, or helical entry move. The entry ramp will be a profile ramp that follows the contour of the cutting pass for a smoother transition into the cut.
- For either type of entry, use the Z clearance to tell Mastercam how far above the previous cut the entry move should begin.
- You can also choose whether to apply the regular feed rate, or the plunging rate to these moves. These rates are specified on the Tool page.
- If you choose to create a helical entry and there is not enough room, Mastercam will create a ramp entry instead.
The difference between these entry moves and the approach/retract moves you define on other parameter pages is that the linking moves connect multiple cuts on the same Z level, while the entry moves control the transition to a new set of cuts on a different Z level.
This page includes additional controls to avoid pockets if they are smaller than a specified threshold. Use them to solve the problem where Mastercam thinks that a pocket is large enough to accommodate the tool, but the entry move is so compressed that the tool is effectively plunging into the part.
- Use Skip pockets smaller than to specify the smallest pocket to consider cutting. Pockets smaller than this value are skipped. A typical value is 110% of the tool diameter.
- Use Preferred profile length to also define the smallest allowable pocket, but as a function of the length of the entry ramp. Mastercam tries to maintain this preference, but this is not guaranteed. In this case, the Skip pockets smaller than field serves as a backup by letting you specify an absolute minimum size that Mastercam does not violate.
| 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
Sets the entry move that the tool makes as it transitions to new Z levels. You can choose to create either a ramp entry, or helical entry move. The entry ramp is a profile ramp that follows the contour of the cutting pass for a smoother transition into the cut.
If you choose to create a helical entry, and there is not enough room, Mastercam creates a ramp entry instead.
Profile ramp
Select this option to create a ramp motion to the next level. Instead of a simple straight line, the tool tracks around the contour of the profile as it moves down to the next level.
Entry helix
Select this option to create a helical entry move between levels.
Radius
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.
Plunge rate
The tool cuts the ramp or helix at the plunge rate specified on the Tool page.
Feed rate
The tool cuts the ramp or helix at the feed rate specified on the Tool page.
Z clearance
This is an extra height 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.
Preferred profile length
Enter a minimum size for the profile in order for a ramp to be created, to ensure that small profiles are not ramped down. Ramping along a very small profile could produce a tight tool motion that would negate any advantage created by the ramp itself. Mastercam tries to maintain this minimum distance but does not guarantee that it can do so in all circumstances.
Skip pockets smaller than
Specifies a minimum pocket size for creating a cutting pass. 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.
- 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.
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.





