Contour Toolpaths: 2D
Use the 2D Contour toolpaths to remove material along a path defined by a chain of curves. Contour toolpaths only follow a chain; they do not clean out an enclosed area. You can select an unlimited number of chains for each toolpath. You can create a 2D, 3D, Ramp, Remachining, Chamfer, or Oscillating type of Contour toolpath.
- 2D cuts geometry in a single
plane (typically XY) at a constant depth (Z), although you can create
multiple passes at different depths. Mastercam automatically defaults
the Contour type to 2D if you only chain
2D geometry.
Tabs are integrated with Contour toolpaths; activate options in the Tabs page (and optionally, the Tab Cutoff page) when creating a 2D Contour toolpath. For more information about the Tab Cutoff toolpaths, refer to the How do I create a Tab Cutoff toolpath? drop-down and for more information about creating tabs, refer to the Using Tabs Help topic.
- 3D cuts geometry in XY and Z, where the Z depth can vary over the toolpath. Use this type if the geometry for each cutting pass is not contained within a single plane. Only available if you chain 3D geometry as part of the toolpath.
- Ramp uses a continuous ramp to transition smoothly between depth cuts, instead of individual plunge cuts. This technique is especially useful in high speed machining
- Remachining calculates areas where the roughing tool could not machine the stock and creates a second toolpath to clear the remaining material.
- Chamfer cuts a chamfer around a corner.
- Oscillating uses more of the cutting length of the tool, and can reduce tool wear in that axis.
You can chain 2D geometry, 3D geometry, or a combination of 2D and 3D geometry for contour toolpaths. Chaining 2D geometry generates a 2D contour toolpath.
If you chain 3D geometry—or a combination of 2D and 3D geometry—you can choose to create either a 2D or 3D contour toolpath.
-
2D contour - offsets and flattens 3D geometry to an absolute depth, relative to the construction plane.
- Absolute depth
- 3D entities
-
3D contour type - offsets 3D geometry with depths matching the chains, then adds the incremental depth value.
- Incremental depth
- 3D entities
When you want to use a continuous ramp to transition smoothly between depth cuts, instead of individual plunge cuts, create a Contour (Ramp). This technique is especially useful in high speed machining. You can ramp by a set angle, by a set depth, or to plunge directly between depth cuts.
To create a Contour (Ramp) toolpath, select Ramp from the Contour type drop-down list in the Cut Parameters page. Then, enter the ramp dimensions in the fields provided.
Remachining calculates areas where the roughing tool could not machine the stock and creates a second toolpath to clear the remaining material. You can choose three methods to calculate how much stock the new toolpath will remove:
- The stock left by all previous operations
- The stock left by the most recent previous operation
- The size of the roughing tool. Use this method when the roughing operation is not included in the current part file; Mastercam determines how much stock would be left based on the size of a roughing tool that you enter.
A low Tolerance creates a more accurate toolpath. For remachining, a low Tolerance may result in more areas being machined.
If you choose Display stock, Mastercam leads you through a series of previews which display the calculated stock to be removed and how much of that stock would be removed with the current remachining settings.
- If you base a Contour (Remachining) operation on a previous operation, and then change the order of the operations in the Toolpaths Manager so that the Contour (Remachining) is before the roughing operation, the Contour (Remachining) will not be able to correctly calculate the area of the roughing operation.
- Do not use compensation in control with Contour (Remachining) .
- Keep tool down moves between remachining passes are not gouge checked! Take the necessary precautions to eliminate the risk of gouging. This applies only if you choose the option to Keep tool down for depth cuts or multiple passes.
- If you use only the previous operation to calculate the remaining stock, and the previous operation is only a finish pass, the Contour (Remachining) toolpath may be cutting air through areas of the part that were roughed by an operation before the finish pass.
Adding oscillation in the Z-axis along your contour toolpaths uses more of the cutting length of the tool, and can reduce tool wear in that axis. This is especially useful when cutting thinner materials or laminated materials such as kitchen counter tops.
When creating a 2D Contour toolpath, you can add an oscillation strategy by selecting Oscillate as the Contour type in the Cut Parameters page.
Then use the oscillate parameters that display below the Contour type field to define your strategy. You can choose a Linear (zigzag) or a smoother High speed (sine curve style) oscillation movement. You also define the Maximum depth and the Distance along contour for the oscillating tool movement.
- The Top of stock that you enter in the Linking parameters page sets the maximum Z height for the oscillating contour toolpath. However, the tool will not exceed the Maximum depth that you specify in the Cut Parameters page.
- The Distance along contour determines how far the tool moves in X or Y before changing direction in the Z axis.
- If you edit the operation and modify the tool, Mastercam automatically verifies that the flute length of the tool is sufficient. A message warns you if the flute length is less than the overall oscillation distance.
You can create a Contour toolpath that only machines chamfers. This toolpath automatically cuts a chamfer around a corner and can be created as a stand-alone operation. To create a Contour (Ramp) toolpath, select 2D chamfer or 3D chamfer from the Contour type drop-down on the Cut parameters page (Mastercam selects 2D or 3D automatically, depending on the chained geometry).
Use the Chamfer parameter in the Cut parameters page to set the chamfer dimensions. Typically, when creating a Contour (Chamfer) toolpath, you set the Depth to 0.0 relative to the chained geometry (on the Linking parameters page), and let Mastercam calculate the tool depth from the chamfer dimensions. Enter a non-zero Depth only if you want to locate the top of the chamfer at a distance from the chained geometry. For example, the following toolpath uses a Depth of 0.0 and a Chamfer width of 0.1. Mastercam calculates the actual tool depth itself:
You must select one of the following tool types when creating a Contour (Chamfer) toolpath:
- Bull-nose cutter
- Ball (spherical) cutter
- Chamfer mill
If you do not select one of these tool types, Mastercam displays a warning after you finish entering the toolpath parameters.
The Tab Cutoff toolpath is a separate operation that you can create when you add tabs to a Contour toolpath. Creating a separate operation lets you edit it separately from the original contour operation. For example, you can select a different tool, or change other parameters such as retract heights, feed planes, lead in / lead out settings for entry and exit moves, or break through amount.
To create a tab cutoff operation, select Separate operation in the Tab Cutoff page while you are entering parameters for a contour toolpath:
Mastercam automatically creates a Tab Cutoff operation and adds it to the Toolpaths Manager. Note that this option is only available when you first create the contour toolpath. If you edit an existing contour toolpath, you can change many of the tab settings, but the Separate operation option will not be available.
Even though the tab cutoff operation is created when you create the contour operation, it does not stay associative with it. This means that if you make changes to the original contour operation, edit its tab settings, or change the tab locations, the changes are not automatically copied to the cutoff toolpath.
However, you can change or edit the tab locations for a tab cutoff operation using the normal tab editing tools. Click on Geometry for the tab cutoff operation to open the Chain Manager. Right-click and choose Edit tabs.
When selecting tab positions, you cannot place a tab on a solid. Tab positions can only be placed on wireframe geometry.
Below are three examples of when you might adjust the start or end of a contour, instead of, or combined with, creating regular lead in/out moves.
The following picture shows an example of this type of toolpath. The toolpath inserts an additional line between the entry arc and the part contour that is at least the width of the tool.

When a contour toolpath has open chains, you can extend and shorten the chains to ensure complete material removal and avoid part walls. The following picture shows an example of this type of toolpath. The lead in/out moves have been turned off in this example.

You can also shorten the contour to leave material behind, like a section that may be cut off by a future toolpath. The following image shows an example of this type of toolpath.
You can also use the tabs feature for Contour toolpaths, which gives you a complete set of tools for creating tabs.
Choose Contour from the selected machine's Toolpaths contextual tab to begin creating the toolpath. After chaining the geometry, you see the Toolpath dialog box where you can enter the toolpath parameters.





