Creating a Mill-Turn Toolpath
Mastercam Mill-Turn is a solution that runs on top of your existing Mill and Lathe licenses. It combines the power of Mastercam's Mill and Lathe toolpaths with a suite of tools and technologies that let you program advanced multi-function, multi-stream lathes and machining centers.
The Mill-Turn platform has specific license requirements depending upon the complexity of the machines being programmed and the user access level. Also, Mill-Turn is not available for Mastercam for SOLIDWORKS. See Understanding Mill-Turn Licenses to learn more.
The workflow for creating a Mill-Turn job is different than other Mastercam products. This is because additional Mastercam tools, such as the Sync Manager, are required to meet the programming requirements of advanced multi-stream machines. In addition, the Mill-Turn workflow is tailored to the specific machine selected for the job. Mastercam loads the proper options, settings, and part handling processes that are specific to the selected machine before the first toolpath is created.
The following outline is a typical example:
- Load the desired .machine file for the machine that you are programming. See About the .machine File to learn more.
- The Job Setup module launches automatically. Select your chucks, jaws, and/or collets tell Mastercam about your stock and part handling needs, and enter the proper dimensions for part stick-out and pick-off positions. Mastercam creates a set of planes with associated work offsets, viewsheets for programming each spindle, and supporting geometry such as turn profiles. See Performing a Mill-Turn Job Setup to learn more.
- Create your turning and milling toolpaths. See Creating a Lathe Toolpath and Creating a Mill or Router Toolpath to learn more.
- When you need to transfer the part to the other spindle, perform a stock pull, or perform a similar operation, select the proper part-handling strategy. Mastercam automatically builds a sequence of individual events that is closely tailored to your specific machine and application requirements. See Part Handling Operations (Mill-Turn) to learn more.
- Set up the tools on your turret. You can let Mastercam do this automatically and edit it as necessary, or do it completely manually. See Tool Setup Manager: Mill-Turn to learn more.
- Finish programming your part in the Sync Manager. This lets you create syncs or wait codes between streams and access custom machine-specific options that have been created for you by your .machine file developer. See Working with the Sync Manager to learn more.
- From the Sync Manager, launch Machine Simulation to preview the machining process and check for collisions. See Working with Machine Simulation to learn more.
- When you have proven out your part and process, post your part from the Sync Manager and generate your NC code. Your post will create the proper multi-stream output for your control, whether it is a single file or separate files. Your NC files will open in the Code Expert Editor, which has a number of tools and features for working with multi-stream NC files. See Working with Code Editor to learn more.
Listed below are the available toolpaths.
These toolpaths are located on the Mill-Turn Turning contextual tab. For more information, refer to the Creating a Lathe Toolpath Help topic.
| Toolpath Name | Gallery Image | Description |
|---|---|---|
| General | ||
| Rough |
|
Quickly removes large amounts of stock in preparation for a finish pass. |
| Finish |
|
Follows the contour of the chained geometry. |
| Drill |
|
Drills into the face of the part. |
| Pinch Turn |
|
Uses two independent tools, located in independent turrets in order to remove material more efficiently. |
| Face |
|
Quickly cleans the face of the part. |
| Cutoff |
|
Vertically cuts off pieces of the part, such as sections of the bar stock. |
| Groove |
|
Machines indented or recessed areas that are not otherwise machinable by roughing toolpaths or tools. |
| Dynamic Rough |
|
Quickly removes large amounts of stock while remaining engaged in the material more effectively, using more of the surface of your insert. |
| Thread |
|
Machines spiral shapes on a part to make a screw, bolt, or nut. |
| Plunge Turn |
|
Creates a toolpath that adds lateral movement to groove-style toolpaths. NOTE
This is designed for special plunge turn tools only, the ISCAR plunge and turn inserts. |
| Contour Rough |
|
Removes large amounts of stock in a pattern offset from part. |
| PrimeTurning |
|
Creates a toolpath for the Sandvik Coromant PrimeTurning method using a CoroTurn Prime tool. |
| Custom Thread |
|
Creates custom thread forms. |
| B-axis Contour Turning |
|
Creates a toolpath that follows the chained contour while allowing for B-axis rotation. |
| Manual | ||
| Manual Entry |
|
Directly inserts text, comments, or G-codes into your NC programs. |
| Point |
|
Moves the tool to a specific point or series of points to avoid a fixture or clamp, or to move the tool through intricate features. |
| Canned (Canned Toolpaths) | ||
| Rough |
|
Creates a roughing toolpath which is based on your machine tool control's canned cycles. |
| Finish |
|
Creates a finish pass which is based on your machine tool control's canned cycles, to finish a canned rough or pattern repeat toolpath. |
| Groove |
|
Creates a groove using your machine tool control's canned cycles. |
| Pattern Repeat |
|
Creates a roughing toolpath in which the cutting passes follow the part contour. |
| Part Handling - Automated (Part Handling Operations (Mill-Turn)) | ||
| Pickoff/Pull/Cutoff |
|
Translates geometry and creates a part transfer operation from the main spindle to the sub spindle and/or a bar pull operation prior to a cutoff toolpath. |
| Pickoff |
|
Creates an operation for the pickoff spindle to clamp onto the part. |
| Stock Pull |
|
Advances the stock material by pulling with the sub-spindle. |
| Tailstock Operation |
|
Repositions the tailstock. |
| Part Handling - Manual (Part Handling Operations (Mill-Turn)) | ||
| Turret Park |
|
Controls the motion of the turret when moving to a parked position. Useful when moving the turret away from the part. |
| Spindle Clamp |
|
Clamps or unclamps the selected spindle. Available settings allow you to set the operation to transfer or eject stock. |
| Spindle Move |
|
Moves the active spindle. |
| Spindle Sync |
|
Aligns the spindles of your machine. |
| Bar Feed |
|
Controls the feed motion of bar stock on a Mill-Turn machine. |
| Manual Tailstock |
|
Repositions the tailstock. |
| Center Point |
|
Creates an operation that uses a center in the turret. |
These toolpaths are located on the Mill-Turn Milling contextual tab. For more information, refer to the Creating a Mill or Router Toolpath Help topic.
Milling 2D and 3D
| Toolpath Name | Gallery Image | Description |
|---|---|---|
|
2D Milling/Routing (2D Mill and Router Toolpaths) |
||
| Contour |
|
Removes material along a path defined by a chain of curves. |
| Dynamic Contour |
|
Uses the entire flute length of the cutting tool to efficiently mill material off walls supporting closed or open chains. |
| Dynamic Mill |
|
Uses the entire flute length of the cutting tools to efficiently mill pockets, open pockets, standing cores, or material left from previous operations. |
|
|
Cleans out material from an enclosed boundary in a finishing or roughing operation. | |
| Face |
|
Cleans the stock from the top of a part to create an even surface for future operations. |
| Peel Mill |
|
Machines between two selected contours or along a single contour. |
| Area Mill |
|
Machines pockets, material that other toolpaths leave behind, or standing bosses or cores. |
| Model Chamfer |
|
Machines safe horizontal chamfers on solid models. |
| Blend Mill |
|
Machines between two open chains. |
| Slot Mill |
|
Machines around closed slots. |
| 2D Hole-making (2D Mill and Router Toolpaths) | ||
| Drill |
|
Machines holes from selected points or arcs. |
| Chamfer Drill |
|
Machines chamfers at the top edge of holes to a specified width or depth. |
| Advanced Drill |
|
Creates a customizable drill operation with different behavior for each segment. |
| Circle Mill |
|
Mills circular pockets based on a single point. |
| Helix Bore |
|
Machines a hole using helical motion based on a single point. |
| Thread Mill |
|
Creates a series of helixes for machining a thread with a thread mill or other suitable tool. |
| 2D Manual (2D Mill and Router Toolpaths) | ||
| Manual Entry |
|
Directly inserts text, comments, or G-codes into your NC programs. |
| Point |
|
Creates a series of tool movements by selecting individual tool locations in the graphics window. |
| 3D Roughing (3D Mill and Router Toolpaths) | ||
| Dynamic OptiRough |
|
Machines very large depths of cuts with a bi-directional cutting strategy to remove the maximum amount of material with the minimum number of stepdowns. |
| Area Roughing |
|
Machines standing bosses and cores, cavities and pockets, or material that other toolpaths left behind. |
| 3D Finishing (3D Mill and Router Toolpaths) | ||
| Waterline |
|
Machines with a series of stepdown cuts along the profile of the selected geometry. |
| Raster |
|
Machines a set of parallel passes with a stepover along a line at a set angle. |
| Equal Scallop |
|
Machines with a consistent scallop motion relative to the stepover distance. |
| Hybrid |
|
Machines steep and shallow areas by utilizing both scallop and constant Z approaches. |
| Pencil |
|
Cleans out material by driving the tool along the intersection of the selected geometry. |
| Blend |
|
Creates motion across or along the selected machining geometry between selected curves. |
| Horizontal Area |
|
Machines the flat areas of the model, creating cutting passes at the Z height of each area. |
| Scallop |
|
Machines the model with a constant stepover. |
| Project (High Speed) |
|
Creates tool motion by projecting selected geometry or an existing toolpath onto the machining area. |
| Spiral |
|
Creates cutting passes where the tool feeds into the part in a continuous spiral. |
| Radial |
|
Creates cutting passes that radiate outwards from a central point. |
Multiaxis
| Toolpath Name | Gallery Image | Description |
|---|---|---|
| Pattern | ||
| Curve |
|
Machines 3D chains or edges. |
| Swarf Milling |
|
Keeps the side of the tool in contact with the selected surfaces or solids, to create a better surface finish quality. |
| Flow |
|
Generates motion along the UV lines of the selected geometry. |
| Multisurface |
|
Machines based on the selected pattern options, cylinder, sphere, or box. |
| Port |
|
Creates a roughing or finishing toolpath for port geometry, machining from top to bottom. |
| Triangular Mesh |
|
Machines where the tool is always in contact with the machining surfaces. |
| Unified Multiaxis |
|
Allows you to select multiple pieces of input geometry to generate the toolpath pattern. Then, using those geometry choices, the toolpath picks the best algorithm to calculate the path. Besides its other uses, Unified can be used to create morph, parallel, along curve, and project curve motion. |
| Application | ||
| Deburr |
|
Breaks edges and removes burrs. |
| Pocketing |
|
Machines with roughing passes for undercuts, wall, and floor finishing. |
| 3+2 Automatic Roughing |
|
Analyzes the part and creates multi-plane roughing operations to efficiently remove material. |
| Rotary Advanced |
|
Creates a 4-axis rotary toolpath that allows for more control over tool motion through the selection of walls, hubs, and shroud surfaces. |
| Rotary |
|
Creates a toolpath along or around the selected rotary axis. |
| Swarf |
|
Creates multiaxis motion that keeps the side of the tool in contact with the selected wall geometry. |
| Port Expert |
|
Cuts a port or internal chamber of a part. |
| Blade Expert |
|
Cuts simple, split, or multi-bladed impellers. |
After creating a roughing operation, users can create an associated pinch turn operation. Users can also easily delete the pinch turn operation and keep the original roughing operation. Mastercam automatically creates all the necessary syncs between the two operations. See Pinch Turn to learn more.
While Mill-Turn uses the same powerful toolpaths as Lathe, the programming environment is more advanced and includes a number of tools to meet the demands of advanced multi-stream machines.
- In place of the single Stock Setup page in Lathe, Mill-Turn includes a detailed Job Setup module. This lets you select and mount workholding components for each job, tell Mastercam about your stock and part-handling needs, and creates a complete set of planes and viewsheets to simplify programming on each spindle.
- A separate Tool Setup Manager gives you complete control over how to organize tooling on each turret. If you wish, you can completely program your turret setup with all of your tools before you even start creating toolpaths. Or, you can let Mastercam do it for you after you have created toolpaths.
- A set of intuitive Mill Setup types uses your Job Setup information to greatly simplify the creation of Mill operations.
- New tools let you create event-based part-handling operations.
- Mill-Turn's Sync Manager application lets you synchronize operations in different streams and access machine-specific options that have been created for you by your machine developer. Use these to provide information to your machine's control that is not available in Mastercam, or to program peripherals like part catchers.
- Component libraries let you create and save libraries of chucks, jaws, collets, and tool locator components. You can then re-use these across different machines or jobs and select which components to use for each part. You can even designate default chucks and jaws individually for each machine.
- Instead of the machine definition–control definition–post architecture used in other Mastercam products, Mill-Turn serializes these resources plus many others into a single .machine file. Hundreds of .machine files are available for purchase, including models for Fanuc, Siemens, and Okuma controls.
- Mill-Turn uses Mastercam's next-generation posting language, MP.NET. This lets Mastercam process multi-stream toolpath data in a robust, efficient, scalable way.
- Mill-Turn offers full Machine Simulation.
See Comparing Mill-Turn and Lathe for a more detailed explanation of the differences between the two products.
The Generate toolpath option automatically generates the toolpath when you click OK. This option is on the pages and tabs of Mastercam's toolpath dialog boxes, and is on by default for new and edited operations. By selecting this option, you no longer need to select Regenerate dirty operations in the Toolpaths Manager after editing your toolpath.
The Generate toolpath option also works with the Apply button on tree-style milling toolpaths. The Apply button applies your parameter changes to the toolpath you are editing without closing the dialog box.
For more information on how this option functions, refer to the Accepting and Generating Toolpaths Help topic.





