Tool Designer for Lathe
Use Tool Designer to create custom 3D lathe tools. 3D tools give you more accurate simulation sessions, often finding collisions that 2D tools do not show. 3D tools also enhance backplotting and verification sessions. The designer comprises many pages of settings that cover every aspect of creating your 3D tool, from loading STEP models to mating an insert to its holder, defining boundaries, setting mounting positions and cutting planes, and more.
To start designing a 3D tool, right-click in the tool selection pane of the operation's Toolpath parameters page, and choose Create 3D tool from the pop-up menu. You can also access Tool Designer by right-clicking in the Lathe Tool Manager, and selecting Create 3D tool.
Hover over any field in Tool Designer to see a tooltip describing that field.
Tool Designer features a top-down work flow, represented by the icons on the left side of the panel. When you first start Tool Designer, the icons represent the two main groups of settings that define a 3D tool assembly. These are the general attributes of the tool and the components of the tool assembly.
To design your tool, start with the Tool page, which is the first set of options, as shown below. When you have filled in the fields on that page, you move down to the next page, Tool Assembly, where you provide information about the tool's components. The following image and list describe each page.
- Tool—On this page, you supply general information about the final tool assembly, including its name, type, tool number, and more.
- Tool Assembly—On this page, you define the components of the tool assembly, including holders and inserts.
The following procedure shows how to create a tool assembly.
-
Click the Tool Assembly icon. The Tool Assembly page displays.
-
In the component list, right-click +(add a component), and choose Define a component from the pop-up menu. The Component page displays.
-
Fill in the values required for your holder. Note that, although there are default values for most of the fields, you must define the Model field before you can move on to the next page of options.
- Move to the next page, Connections, and fill in the appropriate values for your tool. You must define at least the Plane field to move to the next page.
- Move to the next page, Mating, where you can define connections between multiple components.
- Click OK in the Mating page. Tool Designer returns you to the Tool Assembly page.
-
Right-click +(add an insert), and choose Define an insert from the pop-up menu. The Insert page displays.
-
Complete the eight pages of options that define your insert, and click OK in the Insert page. Please see the following section, "Inserts and cutting definition options," for more information on these settings.
NOTE
You can create multiple inserts for your tool assembly. Add additional inserts by right-clicking +(add an insert) and completing the insert definition. -
If you want to create additional cutting definitions for the insert, right-click +(add a cutting definition), and choose Define a cutting definition from the pop-up menu. The Insert page displays, from which you can choose the Cutting Definitions tab.
Inserts and their cutting definitions are the most complex components in a 3D tool. The following image and list describe the many settings needed to define them. For more specific information, view the tooltips that appear when you hover your mouse over a field in Tool Designer.
- Insert—This page holds general insert specifications, such as the insert's name, model, type, and manufacturer.
- Cutting Definition—Each insert can define one or more cutting definitions, which specify attributes such as the corner radius, home position, and cutting side.
- Mating—Here, use the alignment and dynamic transform data entry shortcuts to position the insert in its correct location.
- Setup—Here you specify a plane, rotation angle, offset and up direction for the cutting plane.
- Boundary—On this page, define the tool's boundary and tolerances.
- Machine Orientation—Here you specify the tool's mounting position, turret, tool angle, default active spindle, and spindle rotation.
- Compensation—On this page, you specify compensation values, such as the tool center, the compensation method, plunge and feed direction, and tool clearance.
- Parameters—This page contains cutting parameters, including feed and plunge rate, spindle and cutting speed, and coolant settings.
When importing a STEP file or selecting a solid from the Solids Manager, Mastercam does not import values associated with it. This means, for example, that the Thickness parameter under Shank is not updated for holders or the Corner radius parameter under Dimensions is not updated for inserts.
You must manually update these parameters, or you can use Data Entry Shortcuts in parameters to read values from the imported model.
When modifying the Tool offset number or the Tool back offset number on the Cutting definition page, you may see the parameter box outlined in yellow and a yellow caution message in the tooltip. This message displays when another insert cutting definition already uses the value you entered. It is unusual for tools to share the same offset value. Verify that the offset value you entered is correct for this insert.





