MasterCAM 2020 Step-by-Step Guide
Reference Pages
- 1 1 - Open Template File
- 1.1 Material Based
- 2 2 - Merge Geometry
- 3 3 - Verify Location and Orientation of Geometry
- 4 4 - Define Stock Size
- 5 5 - Roughing Operation(s)
- 5.1 What is a Roughing Operation?
- 5.1.1 Contour 2D - Multi Pass
- 5.1.2
- 5.1.3 Surface Rough Parallel
- 5.1 What is a Roughing Operation?
- 6 6 - Finishing Operation(s)
- 6.1 What is a Finishing Operation?
- 6.1.1 Surface Finish Parallel
- 6.1.2 Surface Finish Contour
- 6.1.3 Surface Finish Shallow
- 6.1.4 Surface Finish Constant Scallop
- 6.1.5 Pocket
- 6.1.6 Contour 2D / 3D
- 6.1.7 Peck Drill
- 6.1 What is a Finishing Operation?
- 7 7 - Adjust Parameters
- 8 8 - Generate Toolpaths
- 9 9 - Verify Operations
- 10 10 - File Approval + Scheduling
Reference Pages
Please use this page in conjunction with the MasterCAM 2020 Reference.
In order to use the large bed CNC routers at the GSD, students must submit a MasterCAM file to the online queue with geometry imported and operations assigned. CNC TA's are available during regular daily hours throughout the semester to answer questions , review submitted files, and run approved files on the mill. This page will enumerate the steps required to have an approvable MasterCAM files.
The GSD CNC lab is not full service. Staff and TA's are not available to set up users' files for them.
The FabLab has created material-specific MasterCAM template files to help alleviate common setup issues.
A basic workflow for successful MasterCAM setup is as follows:
Open template file (material appropriate)
Merge geometry
Verify location of geometry relative to file origin
Define stock size (must match physical material to be milled)
Assign geometry to roughing operation(s)
Assign geometry to appropriate finishing operation(s)
Adjust operation parameters (tool selection, machining heights, etc)
Generate toolpaths
Verify operations (ensure no collisions and desirable outcome)
< repeat steps 4 thru 8 iteratively until successful verification >Submit file to online queue for approval and scheduling
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.
(2020)
(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.
(2020)
(2020)
(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.
| Xmax | Ymax | Zmax |
|---|---|---|---|
ONSRUD | 48" | 96" | 6" |
ROLAND | 12" | 12" | 3" |
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.
Excessive Import Time
Large / complex surfaces or meshes can cause MasterCAM to become unresponsive during merging. This slowdown can be avoided by changing Visibility from shaded to wireframe prior to merging. This prevents MasterCAM from "Tessellating", increasing responsiveness.
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.
| Xmax | Ymax |
|---|---|---|
ONSRUD | 48" | 96" |
ROLAND | 12" | 12" |
4 - Define Stock Size
Reference Pages
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.
Update Machining Heights
After defining stock dimensions, users MUST manually update machining heights to reflect the stock thickness for each operation individually. MasterCAM will not auto-update these values. Inaccurate values cause collisions during verification.
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
Check for Gouging
Note that the Contour 2D operation is not context-aware. Nearby parts may be gouged if there are multiple parts being machined from a single stock.
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).
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
Contour 2D/3D