1 - Open Template File

Material Based

The GSD FabLab provides MasterCAM templates with and without example geometry, for both Foam and Wood projects. It is necessary to separate the two, because the material qualities and behaviors vary greatly and require different tooling and parameters for successful milling.

• The foam template should be used for all densities and types of foams, including extruded polystyrene, expanded polystyrene, and high density polyurethane.

Foam Context Model Milling Template - Without Sample Geometry (2020)

Foam Context Model Milling Template - With Sample Geometry (2020)

• The wood template should be used for all wood and wood products, including softwoods, hardwoods, plywood, oriented strand board, and medium density fiberboard. A special template is provided for milling flat stock materials, such as single sheets of plywood or MDF.

Wood Context Model Milling Template - Without Sample Geometry (2020)

Wood Context Model Milling Template - With Sample Geometry (2020)

Wood Flat Stock 2D Milling Template - With Sample Geometry (2020)

The GSD FabLab does not currently provide templates for less frequently machined materials, though we do maintain tooling to work with the following:

• Non-ferrous metals (aluminum, brass, copper)

• Plastics (Acrylic, HDPE, Corian, Pattern Board)

• Machinable Wax 

2 - Merge Geometry

Preparing Geometry in Rhino

Change Rhino file model space units to inches.

Scale geometry for milling.  

Move geometry to the origin and arrange in all positive space (+X, +Y, +Z).

Check that geometry fits within the maximum machinable extents of the intended CNC mill. 

Explode geometry and remove vertical surfaces.

Note that machinable Z height decreases for tougher materials. 

Organize geometry in Rhino by layer, such that each layer will receive similar treatment in MasterCAM (e.g. Building Tops, Draped Surface, etc).

Avoid using Yellow and Black as layer colors due to MasterCAM interface conflicts. 

Importing from Rhino

Click file in the ribbon menu, and choose merge to open the file picker window. Change the file extension filter to Rhino 3D Files (*.3dm). Select the .3dm that contains your geometry. 

Click open, and the geometry appears in the MasterCAM model space. 

Select the radio button for "Merged File Levels" in the Levels dropdown of the File Merge dialog pane.

Select and then de-select an option from the bottom "Settings' of the Merge Dialog

Press Enter or click the green checkmark. 

3 - Verify Location and Orientation of Geometry

Because the origin of the file typically corresponds to the origin used on the machine, it is important that your geometry be located relative to the origin such that it is appropriately located on the machine. Working far from the World Top Plane Origin in Rhino or similar applications will often cause the geometry to be located far from the origin in MasterCAM, so it's best to catch this issue early, before getting too far along in MasterCAM.

View Work Coordinate System

From the View Tab, choose "Show Axes" and "Show Gnomons"

Verify Location

Your geometry should be located within the positive X, Y, and Z quadrants, with the stock modeled such that it has a corner located at 0,0,0. The gnomon and axes visible on the screen should help to verify whether the geometry needs to move in order to satisfy this condition.

Verify Orientation

Machine dimensions vary, as do the lengths of their respective axes of travel. Make sure your geometry fits within the dimensions of the machine you intend to use.

4 - Define Stock Size

Accurate Dimensions

MEASURE YOUR STOCK

MasterCAM will use the input stock size when simulating, so it is vital to ensure that dimensions are true to the physical material that will be placed on the milling table. 

Entering Stock Dimensions

In the toolpath manager pane, expand the properties subgroup. 

Choose stock setup, and the machine group properties window opens. The stock box is represented by a dashed red rectangular prism. 

Set the stock origin coordinates to 0,0,0. 

Click the lower left corner of the stock box. 

Enter the as-measured dimensions of your stock into the X, Y, Z fields. Default units are inches. 

Tick the display checkbox to show stock box in MasterCAM model space. 

Press ENTER or click  OK to accept the changes. 

5 - Roughing Operation(s)

What is a Roughing Operation?

A roughing operation is used to remove large amounts of material rapidly and to produce a part geometry close to the desired shape. 3D geometry will typically need to include one as the first operation, while 2D geometry may not. A roughing operation uses large diameter tools and coarse settings, and should not cut all the way down to the drive surface(s), instead leaving a small offset for the finishing operations to clean up afterwards. 

Contour 2D - Multi Pass

When stock thickness exceeds the shoulder length of the tools, the surrounding uncut stock may interfere with toolpaths drawn on the perimeter of the part, causing collisions. In this circumstance, it is necessary to partially clear away the stock outside the part perimeter before proceeding to the finishing operations. 

The Contour 2D operation may be used for roughing as follows:

• Assign a part perimeter chain as the input geometry.
• Choose an appropriate tool for clearing a lot of material. Typically 3/4" Flat Upcut Endmill
• Adjust Compensation such that the toolpath is drawn outside the part.
• Enable Multi Passes in the operation parameters.
• Set Parameters > Multi Passes > Rough > Number = 3
• Set Parameters > Multi Passes > Rough > Spacing = 50% of tool diameter.
• Set Parameters > Linking Parameters > Depth to = 50% stock thickness.
• Set Parameters > Cut Depths > Max Rough Step to = 50% flute length

Surface Rough Parallel 

Used to remove material from all surfaces quickly. 

The Surface Rough Parallel operation moves the tool in equally spaced parallel passes in the XY plane across the surface, cutting down incrementally in multiple steps. The toolpath can be drawn as One Way (best for anisotropic materials with grain direction, slower) or Zigzag (best for isotropic materials, faster).

Note that all surfaces except stock extents are assigned as Drive surfaces in a typical MasterCAM file.

6 - Finishing Operation(s)

What is a Finishing Operation? 

A finishing operation follows roughing and is used to achieve the final geometry and surface finish. Most MasterCAM files need at least one and frequently several separate finishing operations to produce an acceptable part. Finishing operations clean up the extra material purposefully left behind by the roughing operation. Finishing operations must be employed on a case-by-case basis, as the utility of each operation type varies from one file (and geometry) to the next. 

See reference pages (linked above) for a detailed explanation of concepts and usage that are common across all operation types. 

Commonly used finishing operations are listed below. Users must review them and determine which operations are appropriate for their geometry.

Surface Finish Parallel

The Surface Finish Parallel operation moves the tool in equally spaced parallel passes in the XY plane across the surface. The toolpath can be drawn in any angle relative to the XY origin. 

This operation is often used with varying stepovers and machining angles to create surface patterns on site models. 

Surface Finish Contour 

Used primarily to clear material from vertical or steep features. 

The Surface Finish Contour operation cuts geometry by offsetting toolpaths away from the drive surface at incremental heights. As sloped geometry becomes steeper, the toolpaths get closer together; as that geometry becomes more shallow, the toolpaths are spaced farther apart. 

This operation is often paired with a flat endmill for use on vertical building faces. Note that the horizontal surface (building top) is the Drive surface.

Surface Finish Shallow 

Used primarily to clear flat areas, such as stepped terrain or building tops. 

The Surface Finish Shallow operation cuts geometry whose slope angle does not exceed a threshold (users can set maximum). 

This operation is often paired with a flat endmill for use on stepped topography and building tops. Users can dramatically reduce machining time by strategically using larger diameter tools to cut open areas, while targeting small diameter tools to narrower channels.

Surface Finish Constant Scallop 

Used primarily to clear sloped areas, such as rolling topography.

The Surface Finish Constant Scallop operation cuts geometry by dynamically adjusting stepover (users can set maximum) as a function of the slope angle for any given point along the drive surface. This method maintains a uniform scallop height across variable relief, and thus uniform smoothness. 

This operation is often paired with a ball endmill for use on rolling topography and gentle slopes. Users can achieve a smoother finish by increasing tool diameter (at the cost of decreasing resolution in narrow channels) and/or decreasing maximum stepover (at the cost of dramatically increasing machining time).

Pocket 

Used to cut flat-bottomed holes, such as building footprints.

The Pocket operation removes material from within a closed chain, creating recesses with flat bottoms. Pockets require closed 2D curves, all in planes parallel to the World Top CPlane. Note that the Pocket operation includes its own internal Roughing and Finishing stages within the parameters. 

This operation is often paired with a flat endmill to cut building footprints. Pockets are preferred over Surface Finish Shallow for cutting deep, flat-bottomed recesses due to their incorporation of incremental depth cuts.

Contour 2D / 3D

Used to trace linear features, such as final perimeter cut-out. 

The Contour operation cuts along a chain or series of chains. The cut may be compensated to the left or right of the chain(s), or on center if compensation is turned off. The chain may be 2D (planar) or 3D. The depth of cut can be absolute (2D only), or incremental (2D and 3D). 

Peck Drill 

Used to create precisely located holes.

The Drill operation creates holes using points as input geometry. Although it is possible to use endmills in a drilling operation, it is preferable to use drill bits. The ONSRUD can accept drill bits of all sizes up to 5/8", while the AXYZ and ROLAND can only accept drill bits in exact collet sizes. 

7 - Adjust Parameters

Surface Rough Parallel

Surface Finish Contour

Surface Finish Shallow

Surface Finish Constant Scallop

Pocket

Contour 2D/3D

Peck Drill

8 - Generate Toolpaths

Drawing the Toolpaths

Once operations have been chosen, geometry has been assigned, and parameters have been adjusted, the next step is to generate toolpaths. Toolpaths are visualized in the modeling space as Blue and Yellow lines that are drawn across the input geometry.

Select the operation(s) that is(are) being used, then generate the selected operation by clicking , or regenerate all dirty operations by clicking .

Dirty Operations

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, parameters, or tool definitions, then the operation is considered "dirty" and the  toolpath icon will instead display . 

The toolpaths for a dirty operation will disappear from the modeling space until regenerated.

If an attempt to verify dirty operations is made, MasterCAM will prompt the user to regenerate with a pop-up dialogue. Verification using dirty operations is inaccurate and should be avoided.

Unused Operations

Delete unused operations to avoid verification mistakes and  

Select the unused operation(s) , then right click > delete. 

9 - Verify Operations

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. 

How to Verify

Select all operations that have been configured and will be used. Operations will be verified in chronological order according to their order in the Toolpath Manager.

Click  verify selected operations in the Toolpath Manager to open the Mastercam Simulator window.

Simulation Playback

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

Ensure that collision checking is activated before starting the simulation:  

• Choose File > Options, then, under General and Collision Checking, check the following within Tool: Stock: Mill tool holder, Mill tool shank, Mill tool shoulder, mill tool cutting length

• Choose Home > Stop Conditions from the MasterCAM Simulator ribbon menu, and then check Collision.

• Choose Home > Tool Components from the MasterCAM Simulator ribbon menu, and then check all items in the Milling field (Holder, Shank, Shoulder, Flute Length).

• Choose Verify > Collision Checking, making sure it is highlighted in blue to enable this function before running the simulation.

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.

Run Time Estimate

MasterCAM Simulator provides an estimate of total run time for selected operations based on specified feed rates, stepover, stepdown, etc. This estimate is displayed in the Move List panel on the right. 

After playing through the simulation, check "Elapsed Time" for the time estimate. Often this estimate is too low by a factor of 2, so as a rule of thumb, double the MasterCAM Simulator time estimate when making a CNC appointment reservation.

10 - File Approval + Scheduling

Complete the Online Form 

Submit a CNC Router Job request online and upload files. Be sure to let us know about any pertinent information related to the job such as material type, your deadline, stock size, or any questions or problems that you've had in making the MasterCAM file. 

Edit Files if Necessary

Once submitted, pay attention to messages in your Microsoft Team as your file is being reviewed. A TA may ask you to meet with them during office hours to discuss what you want to make; they might also ask you to make changes to your file. The status of your submitted file can be viewed through the online queue, along with those of others, but you should also receive notifications as the job status changes.

Schedule Milling Appointment 

After the file is approved, you will be asked to schedule a milling appointment. Visit your job in the queue and choose the "Schedule Job" button to be brought to the scheduler. Choose a block of time that corresponds to the estimated run time for your job, as indicated by the TA in the thread posted to your Microsoft Team.

Prepare Stock Material 

Make sure you purchase and prepare your material prior to your milling appointment (allow 24 hours for most adhesives to fully cure or dry).

Attend Appointment 

You must be present in L33 while the machine creates your part.