Managing Geometry

Merge Geometry 

Rhino (and other CAD) files are imported by selecting File > Merge. This will insert the geometry from the selected CAD file into current MasterCAM file, keeping the same units and origin from the CAD file. Merges are cumulative, and can be performed at any time. 

After the initial merge, subsequently merged geometry will be added to the active level by default. Users may specify to instead merge additional geometry onto the originally assigned level by ticking the radio button for "Merged File Levels" during the merge process.

Select Geometry

MasterCAM breaks apart meshes and polysurfaces into their constituent faces and chains into their constituent segments. The subdivided geometry may be selected piecemeal, or en masse via window selection. Selected geometry turns yellow. Geometry continues to be added to the selection without holding down shift or another key. To deselect geometry, click on it a second time, or press the ESC key to deselect all. The Level Manager can be used to simplify geometry selection by altering the visibility of various levels. 

Move Geometry

Choose "Transform" from the ribbon. Selected geometry can now be manipulated by choosing the desired transformation (Translate, Rotate, Mirror, etc) from the ribbon. Change the Method from Copy to Move, next input the increment of the transformation (units XYZ, degrees, etc). Geometry that undergoes a transformation within MasterCAM will retain its operation assignments, however, the operations will become dirty and require regeneration.

Delete Geometry

Press F5 or DEL to delete selected geometry. If the geometry is included in a toolpath, a dialog box will appear to warn you. To continue, choose “Delete all selected entities”. The selected geometry will then be deleted. Previously associated toolpaths will remain, but will no longer work (they are now "dirty"). 

Visibility

Default MasterCAM view is Shaded. Toggle Wireframe by pressing ALT+S, or choosing View from the ribbon and selecting Wireframe. This will change selectable geometry. Toggle Ghosted display by pressing CTRL+T, or choosing View from the ribbon and selecting Translucency. This will not change selectable geometry. Toggle unselected geometry (show/hide) by pressing ALT+E.

Managing Levels

Layers vs. Levels

MasterCAM geometry can be organized into Levels, which are analogous to Rhino Layers. As with Rhino Layers, Levels may be shown or hidden selectively to allow for easier geometry selection or to decrease visual clutter. Rhino layers will be imported as levels, and the associated geometry will maintain its layer-assigned color. MasterCAM does not use a nested hierarchy for levels, so this organization will be lost when importing from Rhino.

Level Manager

The Level Manager is accessed from Managers pane (defaults to left side of window). Select the Levels tab at the bottom of the pane to see the currently defined levels. The Active Level is designated by a green check mark, and cannot be hidden by default. Click next to a different level's number to make it active instead. Show or Hide levels by clicking the X in the Visible column. Use levels for easy geometry selection by right clicking the desired level's row and choosing Select All Entities.

Managing Planes

WCS + Tplane + Cplane

Each operation generates toolpaths according to the Work Coordinate System (WCS), Tool Plane (Tplane), and Construction Plane (Cplane) that is specified in its parameters. The currently specified planes are also visible in the Toolpath Manager alongside the operation name. The WCS, Tplane, and Cplane should always match for any given operation.

Plane Manager

The Plane Manager allows users to view, create, modify, and delete planes. These planes are referenced by operations in order to draw toolpaths. 

Creating a Plane

In some cases, the default planes may not be appropriate for an operation. For example, the flipped side of a two-sided milling job cannot reference the default Top plane, so a new plane must be created. The most straightforward method is to duplicate an existing plane whose axes are in the preferred orientation, and then enter new origin coordinates for the duplicate plane. 

Managing Operations

What is a Toolpath?

A toolpath is the path through space that the tip of a cutting tool follows on its way to producing the desired geometry of the workpiece. In MasterCAM, toolpaths are represented by blue and yellow lines that are drawn across the surface of your imported geometry. Each toolpath is the result of an operation.

Toolpath Manager

Operations can be created, modified, and deleted in the toolpath manager. It is found within the managers pane, which defaults to the left of the modeling window. 

Hierarchical Organization

The toolpath manager displays information in a file tree format, with the Machine Group as the top-level directory. The machine group contains properties  (contains the machine definition and stock setup) followed by a toolpath group (contains some number of operations). The order of the operations is critical, as MasterCAM will output each in sequence to the simulator, or when the file is posted for running on the mill. 

Operation Components

Within the toolpath manager, operations are displayed as a numbered yellow folder icon with four nested components: Parameters, Tool, Geometry, Toolpath. 

Selecting an Operation

Click on the operation folder icon of the desired operation. Once selected, the operation folder icon will be open and show a green check mark.

Ordering Operations

Selected Operations may rearranged by clicking and holding on the Operation folder icon, then dragging the Operation to a new position within the ordered Toolpath Group. However, it is frequently more precise to manipulate the operation order by using the Insertion Arrow and its controls . The Insertion Arrow exists as a placeholder within the Toolpath Group to allow for the creation of new Operations. The Insertion Arrow can be repositioned by using the Up and Down controls. Once the Insertion Arrow is in the correct position, you may right click on it to create a new Operation, or paste an Operation that was previously copied. 

Toolpath Visibility

MasterCAM defaults to drawing all toolpaths simultaneously in the modeling window. The toolpath for the selected operation can be toggled by clicking . Often it is most practical to only show the selected operation's toolpath while automatically hiding all unselected operation's toolpaths. Toggle this setting by clicking .

Toolpath Generation

In most cases, MasterCAM will not automatically generate the toolpath for a selected operation after its parameters and geometry have been assigned. If the operation lacks assigned geometry, or has had any changes made to the geometry assignment or parameter definitions, then the operation is considered "dirty" and the  toolpath icon will instead display . Dirty operations must be regenerated before verification or posting. Regenerate the selected operation by clicking , or regenerate all dirty operations by clicking .

Defining Parameters

Parameters | UI Inconsistencies

MasterCAM displays parameters for surface-based operations with a tabbed interface, while chain-based and point-based operations use a file-tree interface. Some of the parameters are common across operation type, while others are unique or have multiple names depending on location within the interface.

This disambiguation organizes parameters by the types of operations for which they are applicable.

Parameters | Surface + Chain + Point

Tool Selection

A tool is a piece of cutting hardware that does the actual work of excavating the desired geometry from the stock material. Each tool is a cylindrical piece of metal that has been shaped to perform a particular job. Some tools may be shaped to cut specific materials or give a special finish, while others may be more general purpose. A tool must be assigned to every operation, and each operation may have only one tool. The material-specific template files provided by the GSD FabLab include our default tool libraries. An operation will pre-populate some parameters from the tool library automatically based on the tool selection. The feed rate, plunge, and spindle speed will all be drawn from the library, though these can be overridden by entering a value in the operation parameters. 

The effects of many parameters depend directly on the tool selection, so it is important to update all aspects of an operation's parameters (stepover, stepdown, etc) if the tool selection changes. The tool selection interface resides in a different location of the parameters window, depending on whether the selected operation is surface or chain based. 

Surface-based operations require tool selection on the Parameters > Toolpath Parameters (first tab) page. 

Chain-based and point-based operations require tool selection on the Parameters > Tool subheading.

Planes

Each operation generates toolpaths according to the Work Coordinate System (WCS), Tool Plane (Tplane), and Construction Plane (Cplane) that is specified in its parameters. The currently specified planes are also visible in the Toolpath Manager alongside the operation name. The WCS, Tplane, and Cplane should always match for any given operation.

In most cases, the TOP plane should be specified for all operations. The only exception is when machining the underside of a two-sided job (flip milling). In this circumstance, select FLIP as work coordinate system, tool plane, and construction plane. FLIP plane must first be defined in the Plane Manager.

Surface-based operations allow specifying planes on the Parameters > Toolpath Parameters (first tab) page. 

Chain-based and point-based operations allow specifying planes on the Parameters > Planes subheading.

Machining Heights

During an operation, not every movement of the tool will make contact with the stock material. In between cutting movements (toolpaths shown in blue), the machine must make rapid movements (toolpaths shown in yellow) to reposition. In order to prevent accidental damage to the machined part, MasterCAM requires each operation to specify a safe area where rapid movements will not inadvertently cut through the stock.

Each height value must be specified as Absolute (the input height value is offset from the WCS origin), Incremental (the input height value is offset from the selected operation's assigned geometry), or Associative (the input height value is offset from the defined stock) . Typically, an operation will define a Clearance, Retract, Feed Plane, Top of Stock, and Depth, though some operations may not require every value. 

Surface-based operations accept machining height values on the Parameters > Surface Parameters (second tab) page. 

Chain-based and point-based operations accept machining height values on the Parameters > Linking Parameters subheading.

Parameters | Surface + Chain 

Stock to Leave

MasterCAM allows the user to define an offset, either negative or positive, to be applied between the tool tip and control geometry during an operation. This is useful in a number of situations, but is most commonly used to allow the roughing operation to leave behind a bit of excess material for the finishing operations to clean up afterwards. 

Surface-based operations accept stock-to-leave values for Drive and Check surfaces separately. Users can specify on the Parameters > Surface Parameters (second tab) page. 

Chain-based operations accept stock-to-leave values for floors and walls separately. Users can specify on the Parameters > Cut Parameters subheading. 

Stepover

Operations that clear a broad area typically do so by drawing a trace across the input geometry that the tool will follow, then offsetting some distance to draw an adjacent trace, and so on. This offset distance is called the stepover, and has a direct relationship to the finish quality and machining time of a part. In general, a decrease in stepover corresponds with a decrease in roughness and an increase in machining time. The maximum stepover for an operation should not exceed the diameter of the tool. Stepover must necessarily decrease from this maximum as the density of the stock material, and thus stress on the tool, increases.

Surface-based operations that clear material laterally (Parallel, Shallow, Scallop) require a maximum stepover value to be defined. Users can specify on the Parameters > operation specific (third tab) page. 

Chain-based operations that clear material laterally (Pocket, Contour 2D/3D multi passes) require a maximum stepover (aka "spacing") value to be defined. The location for inputting this value varies by operation.

Stepdown

When the depth of cut required to clear stock material from the control geometry is greater than the flute length of the tool, it is necessary to cut down in layered depth intervals. The height of each depth interval is called the stepdown. In general, an increase in stepdown corresponds with a decrease in machining time, though, the maximum stepdown for an operation should not exceed the flute length of the tool used. Stepdown must necessarily decrease from this maximum as the density of the stock material, and thus stress on the tool, increases.

Surface-based operations that clear material vertically (Parallel, Contour) require a maximum stepdown value to be defined. Users can specify on the Parameters > operation specific (third tab) page.

Chain-based operations that clear material vertically (Pocket, Contour 2D/3D) require a maximum stepdown value to be defined. Users can specify on the Parameters > Cut Parameters > Depth Cuts subheading.

Cutting Method

Surface-based operations that clear material laterally (Parallel, Shallow, Scallop). Users can specify on the Parameters > operation specific (third tab) page.

Chain-based operations that clear material laterally (Pocket). Users can specify on the Parameters > Cut Parameters > Roughing subheading.

This method determines the way in which the toolpaths are drawn across the input geometry. 

Machining Angle

Surface-based operations that clear material laterally (Parallel, Shallow). Users can specify on the Parameters > operation specific (third tab) page.

Chain-based operations that clear material laterally (Pocket). Users can specify on the Parameters > Cut Parameters > Roughing subheading. 

Only applies to One Way or Zigzag cutting methods.

Machining angles allow parallel toolpaths to be rotated relative to the WCS. The default angle of 0 produces toolpath traces with the long direction parallel to the X axis. Increasing the angle rotates the long axis counterclockwise, such that an angle of 90 produces toolpath traces whose long axis is parallel to the Y axis.

Parameters | Surface Only

Depth Limits 

aka "Cut Depths" on Surface Rough Parallel and Surface Finish Contour operations. Users can specify on the Parameters > operation specific (third tab) page.

Constrains cutting moves between minimum and maximum Z heights.

Roll Tool

Users can specify on the Parameters > operation specific (third tab) > Advanced Settings.

Determines whether any portion of the tool is allowed to cut outside the perimeter of the drive surfaces. Defaults is to decide automatically.

Tool Containment

Users can specify on the Parameters > Surface Parameters (second tab) page.

Applicable when containment curve(s) is(are) assigned. Determines how tightly the toolpath is constrained. 

Parameters | Chain Only

Compensation

MasterCAM applies Cutter Compensation when drawing toolpaths based on the input chains. By default, MasterCAM will offset to one side or the other from the input chains by the distance equal to the operation's selected tool's radius. By default, MasterCAM compensates to the  Left or  Right depending on what part of the chain is clicked.

To ensure that all selected chains offset to a particular side, choose Options in the Wireframe Chaining window, then uncheck "Use cursor position" from the Closed Chains field. The Change Side and Reverse functions of the Chain Manager provide additional control over compensation direction.

If the input chains are intended to be centerlines for the operation, Compensation must be turned  OFF

Users can specify on the Parameters > Cut Parameters subheading.

Lead In / Out

Users can specify on the Parameters > Cut Parameters > Lead In / Out subheading.

Commonly used to gradually feed the cutting tool into and out of the stock using line and/or arc elements. This reduces stress on the tool, decreasing overall wear and the chance of breakage.

Multi Passes 

Users can specify on the Parameters > Cut Parameters > Multi Passes subheading.

Creates multiple adjacent toolpath traces from a single input chain. The input chain is offset a specified number of times across a specified distance at the same Z height.

Break Through 

Users can specify on the Parameters > Cut Parameters > Break Through subheading.

An additional negative Z height offset to push the tool through the bottom of the stock.

(Avoid use for best practice. Overlaps with stock-to-leave and linking parameters.)

Tabs

Users can specify on the Parameters > Cut Parameters > Tabs subheading.

Prevents a part from being fully separated from its stock material by leaving behind periodic bridges along the base of a contour cut out. Useful for preserving small parts when using vacuum hold-down, and necessary for all parts when using mechanical hold-down.

Tabs can be generated automatically or manually. When generated manually, users must place the tabs by clicking on portions of the input chain. Tab thickness, width, and ramp angle may also be specified.

Tabs can be moved or deleted individually after creation.

Assigning Geometry

Surface Operations

Most surface-based operations request the assignment of four types of control geometry: Drive, Check, Containment, and Approximate Starting Point. Of these, only Drive is required for toolpath generation, however, it is usually necessary to define additional types of control geometry in order to avoid accidental collisions. Click the geometry component of the selected operation to open the Toolpath/Surface Selection window. In this window, click  to make your geometry selection or click  to clear the previous geometry selection. MasterCAM displays selected geometry in yellow. Press ENTER to save your selection, or ESC to cancel it.

Chain Operations

Chain-based operations use chains as the primary control geometry, but also accept a Start Point for sorting. Some operations (such as Pocket) will only accept closed chains, while other operations will accept both closed and open chains.

Often it is necessary to check each chain once selected to ensure the compensation is in the correct direction. MasterCAM displays this information via four arrows overlayed onto the selected chain. Green arrows indicate the entry point of the chain, while red arrows mark the exit point. The larger green or red arrow indicate the direction of travel that the tool will follow along the chain. The smaller green or red arrow indicates the direction of compensation to be applied to the selected chain. 

Click the geometry component of the selected operation to open the Chain Manager. This window uses its own Insertion Arrow and controls . Right-click within the white portion of the Chain Manager window to bring up the contextual menu. The key functions present on this menu are: Add, Change Side, Sort Options, Delete, Reverse, and Edit Tabs. 

Choosing the Add function brings up the Wireframe Chaining window. There are several options in the Selection Method field that can provide extra control over chain selection. By default, the selection method is set to Chain, but Partial, Window, Polygon, and Single methods may be occasionally useful. 

Point Operations

Verification

What is Verification?

Verification (aka Simulation) is the process of playing out the generated toolpaths in a virtual environment in order to check for errors and omissions. Successful verification (accurate stock and tool definitions, no collisions found) is a necessary pre-requisite to performing any real CNC machining at the GSD. Student submitted jobs will not be approved or scheduled until successful verification is demonstrated. 

Getting Ready to Verify

During Verification, each selected operation will be processed in the order it is placed within the toolpath group; unselected operations will not be processed. Dirty operations cannot be verified, and must be regenerated before verification can commence. 

How to Verify

Select all operations that have been configured and will be used. Next, click  verify selected operations in the Toolpath Manager to open the Mastercam Simulator window.

MasterCAM Simulator

The MasterCAM Simulator creates a virtual environment for testing the validity of selected operations. The generated toolpaths are run in order using the current machine, tool, and stock definitions. It is vital to use accurate tool and stock definitions (representative of the configuration that is loaded onto the CNC machine) for the verification process to produce meaningful results. In addition to visually confirming that the verified geometry matches the designer's intent, MasterCAM Simulator also reports collisions that would result from running the selected operations on the CNC machine with current definitions and parameters. 

The MasterCAM Simulator window includes the simulation environment, the ribbon menu, and the information pane. 

Simulation Playback

MasterCAM Simulator displays simulation progress along a timeline at the bottom of the simulation environment. The timeline is transparent, but becomes opaque on mouse hover. Toggle the simulation playback by pressing R or clicking the play/pause button. Users can scrub backward and forward along the timeline by clicking and dragging the red slider, or incrementally by pressing B (backward) and S (forward). Users may skip to the previous or next operation by pressing P (previous) and N (next). Users may skip to the start or end of the job by pressing HOME (start) or SPACE (end). 

Collision Checking

Collisions occur when any portion of the CNC machine or tool that is non-cutting comes into contact with the stock material. Ensure that collision checking is activated before starting the simulation. First, choose Home > Stop Conditions from the MasterCAM Simulator ribbon menu, and then check Collision. Next, choose Home > Tool Components from the MasterCAM Simulator ribbon menu, and then check all items in the Milling field (Holder, Shank, Shoulder, Flute Length). Finally, choose File > Options and then enable all Collision Checking options for Stock and Mill Tool (Mill tool holder, Mill tool shank, Mill tool shoulder, Mill tool cutting length).

During simulation playback, areas of the stock involved in a collision will be colored dark red. The type of collision can be identified in the Collision Report.