Cut Parameters: Dynamic Milling
Use this page to specify cutting parameters and compensation options for a Dynamic Mill or Dynamic Contour toolpath. This includes defining a microlift distance, retract moves and stock to leave. Microlifts raise the tool slightly off of the part on back moves (non-cutting moves) to help clear chips and minimize excessive tool heating. The Cut order optimization drop-down allows you to control where you start a new cut within a pocket. By default, it is set to Material, which starts at the most recently machined material.
Use the pages nested below the Cut parameters page to activate and configure advanced toolpath features. These additional parameters may include depth cuts, contour walls, finishing, entry motion, and break through amount.
Not all options are available for all toolpaths.
| 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. |
Cutting method
Orients the cutting direction. Select one of the following options:
- Climb: Cuts in one direction with the tool rotating in the opposite direction of the tool motion.
- Conventional: Cuts in one direction with the tool rotating in the same direction as the tool motion.
- Zigzag: Cuts each pass in the opposite direction to the previous pass. A short linking motion connects the two ends.
Compensation direction
Offsets to the tool based on the selected direction. Choose one of the following:
- Left: The tool is allowed to travel to the left of the selected chains.
- Right: The tool is allowed to travel to the right of the selected chains.
Tip compensation
Select whether the compensation point will be the center of the tool or the tip. Compensating to the center of the tool is frequently used with ball cutters where compensation is applied at the control.
Approach distance
Adds an additional distance to the beginning of the first cut. Enter the distance as a percentage of the tool diameter or as an absolute distance. Use the drop-down to select the location of the approach.
First pass offset
Offsets the machining region to ensure the tool does not engage too much material during the first pass of the toolpath entering stock from the outside.
First pass feed reduction
Reduces the feed rate of the first pass of the toolpath entering stock from the outside.
Conventional feed rate
Sets an alternate feed rate for the conventional motion of a zigzag cut. Enter a percentage of the programmed feed rate or a value.
Stepover
Sets the distance between cutting passes in the X and Y axes. Enter a percentage of the tool diameter, an absolute distance, or an angle. The value or percentage is limited to 95% of the tool's flat diameter. A larger value will automatically be reduced to the 95% limit after a warning message. Be aware when using a bullnose tool that the percentage is a calculation based on the tool's flat diameter.
The field becomes a drop-down selection when the following conditions exist:
- An ISCAR CHATTERFREE tool is selected
- The Iscar HEM checkbox in the Tool page is selected
Your options then become 5%, 7%, and 10%.
Minimum toolpath radius
Enter the minimum toolpath radius to create in the operation. Enter the value as a percentage of the tool diameter or an absolute value. Mastercam uses the specified minimum toolpath radius in combination with the Microlift distance and Back feed rate parameters to calculate 3D arc moves between cut passes. The Minimum toolpath radius value is beneficial when the following conditions are present:
- Sharp corners in your machining chain: If you machine a rectangular-shaped pocket, each of the four corners will have a radius. The Minimum toolpath radius is the radius of those corners.
- Arc on and off: The arc motion on and off during toolpathing tries to target 45% of the tool's diameter for its size. However, if the percentage prevents the tool from going into a tight space, Mastercam makes this value less than 45%, but never less than the Minimum toolpath radius value.
Keep tool down within
Prevents the tool from retracting between passes.
- Distance: If the distance from the end of one pass to the start of the next pass is less than this distance, Mastercam will not create a retract move as defined on the Linking Parameters page. Instead, the tool will stay on the surface and move directly between the passes at the feed rate.
- Percent of tool diameter: If the distance from the end of one pass to the start of the next pass is less than this distance, defined as a percentage of the tool diameter, Mastercam will not create a retract move as defined on the Linking Parameters page. Instead, the tool will stay on the surface and move directly between the passes at the feed rate.
Motion < Gap size, micro lift
-
Micro lift distance: Enter the distance the tool lifts off of the part on back moves. Microlifts are slight lifts that help clear chips and minimize excessive tool heating.
- Back feed rate: Controls the speed (inches per minute or millimeters per minute) of the tool's backfeed movement. This allows 3D arcs between cuts to have a different feed rate than the rest of the toolpath, which can help reduce cycle time.
Micro lift retract
Controls retracts in the toolpath when making a non-cutting move within an area where the tool can be kept down or microlifted. Choose one of the following options:
- Never: Eliminates retracts from the toolpath for these types of tool moves.
- Avoiding a boundary: Adds retracts to avoid intersecting boundaries (a gouge boundary, or a boundary of material yet to be milled). The types of boundaries that Mastercam detects and avoids include chained geometry, part features, and stock.
- Exceeding a distance: Adds retracts when the next cut pass begins at a distance that is greater than the distance you define, either as an absolute Distance or as a Percent of tool diameter. The distance is the allowable length of the down or microlifted move.
Choose options that include boolean expressions (OR/AND) to further customize retract moves for your application.
Cut order optimization
Controls the cut order Mastercam applies to different cutting passes in the toolpath. When the tool finishes a machining pass, it must select a start point to resume. The start points can be set as the following. The images below show a toolpath with Classic Backplot to help show the differences between the options. The numbers indicate the order of machining to also help visualize the options.
-
Material: Set by default. Starts at the material that is closest to the entire tool. Mastercam attempts to do smaller pieces within a general area when pieces of material become isolated before moving on.
-
None: No optimization is applied to the cutting passes.
-
Air: Starts nearest to the tool. Mastercam attempts to create the shortest possible air moves between machining areas.
Stock to leave on walls
Sets the amount of stock on selected vertical machining geometry. Enter a positive value if you do not want to remove all stock or enter a negative value to remove more stock. If the machining geometry (or a portion of it) is not vertical, Mastercam interpolates a value between the Stock to leave on floors and Stock to leave on walls amounts.
Stock to leave on floors
Sets the amount of stock on selected horizontal machining geometry. Enter a positive value if you do not want to remove all stock or enter a negative value to remove more stock. If the machining geometry (or a portion of it) is not horizontal, Mastercam interpolates a value between the Stock to leave on floors and Stock to leave on walls amounts.





