Cut Parameters: Peel Mill
Use this page to define the cutting parameters used to create a Peel Mill toolpath. The toolpath is created using dynamic tool motion along a single selected chain, or between two specified chains (two chains are used in the following illustration). Dynamic motion allows the toolpath radii to change based on the part. Instead of a full radius between passes, the radius is altered to reduce excess motion.
Mastercam's microlift parameters help to clear chips and minimize excessive tool heating. When microlift is active, the tool lifts slightly off of the part on back moves, using the specified feed rate.
| 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 style
Sets the cutting style for the toolpath. Choose one of the following options:
- Dynamic peel: Use this option to machine areas by using an open chain. This cutting style uses a dynamic style of motion with accelerated back feed moves when the tool is not engaged in material.
- Peel: Use this option to machine areas by using an open or closed chain. This cutting style uses a trochoidal style of motion with accelerated back feed moves when the tool is not engaged in material.
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.
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.
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.
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.
Extend Entry/Exit
Use these fields to adjust the initial and final tool engagement with the material. Select the checkbox to active the option, then enter an Additional entry/exit distance. By default the initial cut is defined by the stepover amount. Mastercam adds the additional amount you specify to the beginning and/or end cut. These options are useful if the part geometry between the two chains is something other than a straight line, such as a slot that spans the corner of a part.
Extend entry off:
Extend entry on with an applied extension value:
Single chain only
Available when a single chain is selected for the toolpath. Sets the orientation of the toolpath along the selected chain.
- Choose Center to align the tool center with the centerline of the chain.
- Choose Left or Right to offset the tool center by the tool radius along one side of the selected chain. The left and right sides are defined by the chaining direction.
- Sloth width: Enter the total width of the slot to cut (the width of the cutting area for the toolpath). Mastercam drives the toolpath along the single chain using the selected toolpath orientation (left, center, or right).
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.





